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History-vs-Non History based CAD softwares
8

History-vs-Non History based CAD softwares

History-vs-Non History based CAD softwares

(OP)
Does anybody have any good articles where they have compared history based -vs- Non history based CAD software??? Primarily I was lloking for productivity benchmarks. Any help would be great. Thanx.

Brad

RE: History-vs-Non History based CAD softwares

Can you clarify for the simple folks such as myself what you mean by history and non-history based CAD software?

RE: History-vs-Non History based CAD softwares

2
I think it as mainly to do with your kind of work.

In an history-based CAD you have a very well structured model creation and you can always go back to modify it.

If you develop new products/components, it is very important to have access to the history so you can make "what if?", optimize, ... and maybe the most important, have a design intent. I am shure that these CAD's have important features (in the development point of view) not available in non-history CAD's - I think configs will be one of them.

In non-history you only have the final geometry available. You loose track of all the features used so far. You can only modify the model by adding geometric operations.

Non-history based CAD that I know are very focussed in design. In this case the most important is to have the final geometry and a light file.

Regards

RE: History-vs-Non History based CAD softwares

History= feature driven models
Non-history= no features

"I think there is a world market for maybe five computers."
Thomas Watson, chairman of IBM, 1943.
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RE: History-vs-Non History based CAD softwares

3

http://www.amrcc.com/pdtt/cad.asp

History vs. Non-history based

In a history based system, the program remembers the order that features were constructed in, non-history does not. For instance in a history based system (ProE, SolidEdge, etc.) let's say cylinder A is built first, then block B is built on the face of the block, then a boss C is built on a face of block B. In a history based program block B cannot be deleted leaving only cylinder A with boss C attached to it. The program remembers that boss C was built after block B and was attached to it. If block B is removed the system no longer has a feature or face to attach boss C to and the model regeneration will fail.

Tools with the ability to manipulate the history tree are usually supplied with these software's to allow the operator to trick the system by moving a feature to an earlier point in the history tree (telling the system that boss C was created before block B). This step may or may not allow the part to regenerate. Also, if the feature you want to remove was created early in the modeling of a complicated part, you may have to do extensive manipulation of the tree in many steps to allow you to make the desired change. In a non-history based system (CoCreate SolidDesigner) the software makes no distinction between which feature was created first. Modifications are allowed in any order.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

Do you trust your intuition or go with the flow?

RE: History-vs-Non History based CAD softwares

Rhino is non-history.  For some reason, a lot of other industrial designers seem to like it.  I can't stand it, since nothing I design remains unedited.  So changing something means a long series of "undo" commands, or rebuilding entirely.

I have no idea what the advantage to that is (software price, perhaps), but I've had clients who design everything in Rhino, then pay me lots of cash to rebuild it in SolidWorks.  Quite a waste of time and money, and that doesn't include all the rebuilding they had to do to get their final model within Rhino.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: History-vs-Non History based CAD softwares

bcoutermash ... If you can find out which programs use which method, you may have more luck finding performance comparisons via names, rather than via History vs Non-history.
 


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RE: History-vs-Non History based CAD softwares

Kubotec KeyCreator (formerly CADKey) talks about it a lot in their user newsletters and marketing.
However, for an experienced user, I think it comes down to preference.  Some users will state that a history based program is more constraining and can lead you into situations that you can not edit your way out of without ruining the model geometry.
On the other hand I find it more troublesome to remove holes in a pure geometry modeler by having to fill them in with more solids.
Certainly the more flexible a history based modeler is, the better off you are.
SW training pushes `Design Intent' which can be good for downstream applications, multiple revisions, or components that eventually get edited by multiple designers.
If you are well trained, and each item is a custom piece, some will argue that you can be faster with a pure geometry modeler.

DesignSmith
www.DesignSmith-Services.com

RE: History-vs-Non History based CAD softwares

To go a bit further related to my earlier post, all "standard" CAD's for mechanical design (SW, SE, CATIA, PRO/E,...) are history based. I could not think working any other way. Like Theofilus complaint, it would be almost impossible for us to do mechanical design using a non-history CAD.

Rhino it's one CAD (should we call it CAD?) devoted mainly to insdustrial design. It don't have feature history. I could say (correct me if I'm wrong) that all CAD's devoted to industrial design don't have it.

From what I have seen, these industrial CAD's are better than mechanical CAD's in the following aspects:
- simple modeling of free forms, nurbs,...,
- better rendering tools and more realistic results
- model files are smaller
- less hardware demanding

So, in my opinion, more than performance comparisons, it will be your work that will define the type of CAD you should use. Basicaly: machanical design/history CAD (necessarily); industrial design/non-history CAD (maybe).

Regards

RE: History-vs-Non History based CAD softwares

I'm not sure.  Alias Studio probably has history, but I haven't gotten into it far enough to know--it's more expensive than SW and is aimed squarely at the ID market.

The big thing I cannot justify is when the non-history part/surfaces are handed to the engineer (from, say, an industrial designer) and the surfaces must either be imported--and never changed--or the file must be completely rebuild (and therefore interpreted) by the engineer.

Since SolidWorks has increasingly powerful surfacing capacity--and since I'm an industrial designer--there's no way I would justify paying industrial designers for the convenience of quick-but-useless NURBS surfacing when I'll need to pay engineers to rebuild everything.  Many region's markets just won't handle that sort of bloated budget anymore.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: History-vs-Non History based CAD softwares

For those who have not seen or dealt with non-history based CAD programs, take a look at the following URLs. I had to use Internet Explorer for the Co-Create demos to run properly.

http://www.cocreate.com/OSDM_overview_demo.cfm#
http://www.ironcad.com/product/overview.html

I used Co-Creates Solid Designer (now totally revamped and called One Space Designer [OSD]) for 4+ years before switching to SW. It is a great program, but probably no quicker or easier in the initial creation of a model than with SW.

It does however, excel in two main areas:-
1) when  changing a feature of the model ... With history based CAD, when you edit a feature which was created early in the tree, all the following features get suppressed, so you are unable to reference them or even use them as approx guides. With OSD, you can reference any feature at any time.
2) when importing other CAD models ... Because non-history does not concern itself with "features" & their pecking order, there is no such thing as a "dumb solid". A parasolid file can be imported & worked on as if it had been created with the non-history program or as if a "Feature Recognition" module had been used ... but without sketches being created.
An interesting thing with OSD, is that once a feature has been created, the sketch & plane used to create it can be deleted. The program recognises the geometry of the created solid feature.

Quote (DesignSmith):

I find it more troublesome to remove holes in a pure geometry modeler by having to fill them in with more solids.
With OSD you do not have to fill in the hole ... you simply "cut" (delete) the surfaces involved from the model & the surface containing the hole "self heals".

Both History & Non-history have their own strengths & weaknesses. Imagine a shaft with three reducing diameters of  say, 3", 2" & 1" (3 features). With OSD, if you change the 2" dia to 3",  the shaft becomes built of two features. Great if you want to minimize the "feature tree" (yes ... it does have one if you want to view it but usually you don't need to) but not so great if you want to reduce the diameter back to 2". You have to do another "cut-extrude" to reduce it.

bcoutermash ... Don't believe all the negative propagnda you will hear from the Non-history CAD vendors. Having used both SolidWorks & Solid Edge, IMO the History based ones would  hold their own in a head to head contest. If you do  find any definitive comparisons, please post them here for future reference.


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RE: History-vs-Non History based CAD softwares

CBL - Perfect explaination.  But self heals sounds like a Microsoft product

Quote (CBL):

With OSD you do not have to fill in the hole ... you simply "cut" (delete) the surfaces involved from the model & the surface containing the hole "self heals".

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

Do you trust your intuition or go with the flow?

RE: History-vs-Non History based CAD softwares

1 program I haven't seen mentioned is the Ashlar line of products: Vellum Solids, Cobalt, ect..

They're sort of a hybrid history based/non-history based software.  You can go into the design tree and see the order in which things were created and modify them that way.  Esentially the same as SW.  Or you can just select the remove tool and pick a hole, fillet, boss, whatever and delete it w/o regaurd for when it was created, or how it was created.  You can also do the same thing with the move or other tools.  Later if I wish to readd the hole it's as simple as deleting the remove command out of the history tree.

One function I greatly miss when doing design work is being able to simply pick a face of a solid and extrude it, or contract it.  Or circling part of a part and extending or shortening it simply by dragging (ie making a 3" plate 2" or 5").  Being able to extend/contract any face of a plate w/o regaurd for how it was created is much faster, and much more versital.  Particularly on parts I didn't draw; where it often takes a lot of searching through the design tree to figure out how something was created before I can figure out how to modify it.

Best of both worlds.  I find only having the design tree method to be extremely constricting.  Keep hoping SW will add the other functionality to their software.

Can't say I understand why we have to choose history/non-history based.  Seems kind of like choosing power steering or power brakes, but not both when buying a new car.

RE: History-vs-Non History based CAD softwares

When changing a feature in SW, you don't always have to use the Feature Manager. You can double click the feature in the graphics area to display (usually) all the dimensions controlling that feature, then simply change the dimension.
Similarly, for deleting features, simply highlight the feature in the graphics area & hit the "Delete" key. This however is history dependant & will  remove all dependant child features.

Quote:

Later if I wish to readd the hole it's as simple as deleting the remove command out of the history tree.
So all it's really doing is the equivalent of SWs "suppress" feature, but without the "complication" of adding yet another icon into the tree.


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RE: History-vs-Non History based CAD softwares

So all it's really doing is the equivalent of SWs "suppress" feature, but without the "complication" of adding yet another icon into the tree.

Not exactly.  you could go into the history tree and suppress or delete the hole that way, much like SW.  The advantage is you can simply select the holes on the solid model and remove them.  Let's say you have a plate with 120 holes in it. In SW you have to go through the history tree and figure out which feature the holes are part of (there could be 120 hole features, or the 3 holes could be in 3 different features).  Then you have to edit each feature once identified, perhaps edit them in different ways depending how the holes were created.  Lots of steps, lots of time.

Vellum select the tool, select the 3 holes, done.  4 clicks, maybe 15 seconds.

{When changing a feature in SW, you don't always have to use the Feature Manager. You can double click the feature in the graphics area to display (usually) all the dimensions controlling that feature, then simply change the dimension.}

I do like that feature.  Works good sometimes, except, if you need to add or subtract off an extrusion it's only useful if the end you wish to change happens to have been extruded the right way (again history dependant).  I've found nothing similar in SW to just being able to select the face and extrude it or subtract it.  Example, I just needed to add 3"  to a structural pipe. Couldn't just add 3" because it was extruded midplane.  Well I needed 3" on end B not 1.5" on each end.  Rather then mess with a lot of mates, moving mounting holes, ect. I redrew the profile and added on.  Worked ok, but many steps instead of a couple.  Vellum I'd select the tool, select the face, drag in direction desired, type in distance desired, hit enter, Done.

Which reminds me, why when you convert edges of a face does SW only convert the outside profile?  If you want to also convert any other details you have to individually select those items then convert them.  Usually I also want the holes, ect on the face, not just the profile.

RE: History-vs-Non History based CAD softwares

SW added the right-click option of "select loop" and "select tangency".  I like this better than automatically converting all the stuff inside the outer profile, since most often I don't want to covert everything inside anyway.  Useful new feature I get a lot out of now that I've discovered it.  (Much  better than in 1997 when I learned SolidWorks.)

By the way, perhaps part of the reason SW doesn't combine history and non-history capacity is legacy stuff.  Back in 1996 when SW was being brewed, one was lucky to have a 133 MHz Pentium chip driving their system.  Resources were treated as the scarcity they were.  I would imagine lots of the code was driven for efficiency, and therefore hasn't been split to include the history/non-history feature capacity for that reason.  (And that there probably hasn't been a clamor from the user base for such functionality since SolidWorks is gold when compared to ACAD and other traditional CAD packages.)


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: History-vs-Non History based CAD softwares

ongybill ... good points & good examples.


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RE: History-vs-Non History based CAD softwares

Quote (ongybill):

Example, I just needed to add 3"  to a structural pipe. Couldn't just add 3" because it was extruded midplane.  Well I needed 3" on end B not 1.5" on each end.  Rather then mess with a lot of mates, moving mounting holes, ect. I redrew the profile and added on.  Worked ok, but many steps instead of a couple.

... just realised, with your tube example, if you RMB the graphical feature you can select Edit feature & change from mid-plane to Blind & set Direction1 and Direction2. That's still several more steps than with Vellum but beats having to add another feature to the tree. OSD has a similar function & I really like that.


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RE: History-vs-Non History based CAD softwares

Quote (ongybill):

One function I greatly miss when doing design work is being able to..<snip>..circling part of a part and extending or shortening it simply by dragging (ie making a 3" plate 2" or 5").  

Look up "Move/Size Features" in Help . . .

RE: History-vs-Non History based CAD softwares

ongybill

Is Ashlar, an history based CAD? With your posts, it seems to me that you are talking about some kind feature organization, but not an history based CAD.

In history based CAD, you have a parent/child relationship. Picking your example of selecting several holes at once and deleting them, that can be very simple in SW, depending on what type of model and modeling technic you are using (design intent). If you are practicing good modeling and you are not able to select all holes to delete, it's probably because it was ment to be that way. There are difterent holes, with different parent/child relationship and there's no reason to delete them at once. That can even cause the part to fail to rebuild.

On the other hand, holes of the "same family" should be modeled in a way that any modification (new dimentions, suppressing, deleting,...) would be easy to do, otherwise will have a case of bad modeling.

In SW you can also organize features in folders and rename them in order to make the model more easy to handle. A model with tenths of cuts, extrudes and paterns will be very hard to handle. But if organized in folders and/or with meaningful feature names it will be very easy.

I don't think that's a case of choosing power steering and power brakes. It seems to me that you can't have a car in clear black. It can be clear, it can be black, but not both. And that does not mean that the clear car will be better or better used than the black one. Just drive the one that suits you better.

Regards

RE: History-vs-Non History based CAD softwares

CorBlimeyLimey
{... just realised, with your tube example, if you RMB the graphical feature you can select Edit feature & change from mid-plane to Blind & set Direction1 and Direction2. That's still several more steps than with Vellum but beats having to add another feature to the tree. OSD has a similar function & I really like that. }

Good suggestion, never thought of doing it that way.

??What does OSD stand for??

MElam
{Look up "Move/Size Features" in Help . . .}

Thanks for the suggestion.  I tried it and couldn't get it to work, probably because I was in an assy and it talks of multi-body parts.  Or perhaps because the parts were fully defined.  If either of those guesses are right it's a very limited, but still useful tool (I don't do many multi-body parts).  But, I'll play with it later and see if I can figure out how to make it work.  I try to learn a new command a day, that's a good one for today.

RE: History-vs-Non History based CAD softwares

OSD = One Space Designer (formerly Co-Creates Solid Designer)
See my post on 7 May 05 23:16


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RE: History-vs-Non History based CAD softwares

macPT
{Is Ashlar, an history based CAD? With your posts, it seems to me that you are talking about some kind feature organization, but not an history based CAD.    In history based CAD, you have a parent/child relationship.}

I'd say Ashlar is more flexible.  I'm not a programmer, & I'm not sure the full definition of history/non-history based.  I'm also 6 years out of date with Ashlar's software.  But, the older software is more of an either/or proposition.  You can work as history based, or you can simply draw what you want w/o paying any attention to the history, or you can do a combination (the history's there if needed).  I used it mostly when I wished to resize holes.  Ocassionally, I find history based to be superior.  Most of the time it's slower, more tedious, more steps, more time.  I seldom used that feature in Vellum for this reason.  Same way I seldom used dimension or equation based sketches to draw something.  Ocassionally useful and superior, but unneeded for most of what I draw.

You can add parent/child relations when they're helpful, or if you want to, but you aren't forced to (I think you can set it to do so automatically like SW, but not sure).  Which I like as I find parent/child to cause more problems then they solve in most cases.  I know Ashlar's newer software allows you to use constraints, but doesn't force you to all the time like SW.  Constraints again are a useful tool (something I really missed w/ Vellum), but not all the time.

Also I find SW models are much more fragile.  You mentioned not deleting holes right and causing rebuild errors.  For me that's a new one.  Not used to models being so fragile.  I get models all the time from our engineers that have obsolete parts in the assys.  They're afraid to delete them because they'll likely create errors if they do.  I just kept a part in a large assy for the same reason.  Everytime I deleted it it caused massive problems.  Couldn't figure out any way around that, so for the first time in years I deliberately left a part in a fixture that doesn't exist in real life.  Lousy practice and not something I'm happy about (likely to confuse someone down the road), but. . . .  

When I started using SW having people tell me well you drew that wrong remodel it this way and it'll work surprised me.  I haven't scrapped a model and started over because I didn't create it properlly since Autocad.  Though I've done it quite a few times this year.

I'm finally getting proficient with SW, though I have tons to learn still, but I'm more convinced all the time that in many signifigant ways it's inferior to Ashlar's software, at least for me.

Organizing things is slightly different in Vellum.  You don't put them in folders, but you can group them together, or put them on the same layer, or add parts together, or other ways of organizing things.  Of course an assembly is one file, not a file for each part as SW does it.  It's definately a different animal.

I see SW more of your car is black, clear is NOT an option, so just deal with it.<G>  Like being forced to start every part as a 2D sketch (no 3D drawing allowed).  

For me at least, SW is an OK tool, far superior to what I used in college 12 years ago, but definately not what I'd choose if I had the choice.

Well, probably more then you wanted, and I'll probably get reamed for saying SW is inferior to anything in any way, but just 1 man's opinion.

RE: History-vs-Non History based CAD softwares

ongybill, are you more of an engineer or an industrial designer?  I would guess ID, based on the non-legacy flexibility you indicate as your preference.  Good post.

Just as the history can be somewhat constraining, it can certainly be used to be much more powerful--moving from a hindrance to an asset.

For instance, I modeled a single part with seven solid bodies and lots of surface bodies through over 450 features.  That was a complex part (injection molded housings) that will be broken into separate components.  It would have been impossible for me to create that part (feasibly) without reliance on history.  Hundreds of times I had to move up the tree (back in time) and tweak a value to change things deliberately downstream.  If I can double-click a dimension, or simply move a feature backward or forward along the process, this can be incredibly powerful.

The difficulty is that training a mind to build models in such a way is difficult and slow.  It comes down to a logical process such that edits can be made easily without the catastrophic results you mentioned.  I faced that all the time when I learned SW back in 1997.  I kept finding myself wondering why the confounded software wouldn't allow me to perform a particular operation, only to figure out what I was trying to do was geometrically irrational and therefore logically impossible.  (So I wasn't having difficulty with the software, but the laws of reality.)

Meanwhile, the history stored in the feature tree can be used such that the poor practices you mentioned (and I agree with your assessment) aren't necessary--within assemblies or parts--but the modeling does need to be done according to rather strict practices.  I can't stand having corrupted parts or features in models as necessary legacy.  They can always be removed, but if the modeling was done poorly (or merely without foresight as to how the models would be used in their current context), the time is sometimes not justified to correct the bugs.

Since the mode of thinking is so much different with history-storing models, it will take some time and practice to make it work to your advantage instead of to your detriment.  That comes with the proficiency you mentioned and I think you'll find it useful down the road.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: History-vs-Non History based CAD softwares

{ongybill, are you more of an engineer or an industrial designer?  I would guess ID, based on the non-legacy flexibility you indicate as your preference.  Good post.}

You would be right, though I also do a great deal of design work. I spend a great lot of time doing parts drawings of complex assemblies.  Design intent, parent/child, & history is just time consuming nonsense when all I wish to do is draw widget Y purchased from company X.  I just want it close to the correct size, with accurate mounting features, as quickly as possible.  The rest of it's useless as I'm never gonna build the part, and it's not possible to tweak the size.

Of course even in my design work, the legacy flexibility is of limited usefulness as so much of what I do is custom work.  Meaning there's little chance of building that part again, and there's seldom a family of similar parts to worry about.  So while useful, it's of limited usefulness to me personally.

{The difficulty is that training a mind to build models in such a way is difficult and slow.}

I'd certainly agree with this statement.  I find much of SW to be totally counter-intuitive.  Such as starting all 3D models as 2D sketches.  Not sure I'll ever understand why it works that way.  In fact I wasted a great deal of time up front because I found it so difficult to believe that was actually how things had to be created.  But, after much searching I've accepted that SW isn't a 3D drawing program, at least not in the way I'm used to.

{Since the mode of thinking is so much different with history-storing models, it will take some time and practice to make it work to your advantage instead of to your detriment.  That comes with the proficiency you mentioned and I think you'll find it useful down the road.}

True, I'm gradually finding it more useful.  Just would prefer not to be forced to use it most of the time when it's a detriment not a help.  Perhaps someday my thought processes will get warped into SW mode & it'll make sense.<G>  Now it's just a bunch of unnecissary steps SW needs because it wasn't set up very well to begin with.  

It'd also help tons if the tree didn't act like a possessed slinky.  Maybe there's some logic to how it expands and contracts which parts are open and where on the tree it is, but I can't figure it out.  I hate when I wish to modify the mates of part X and I have to keep refinding and reopening the correct folders in the tree.  Or worse accidentally modifying the wrong part because it closes part X and opens window on part X(2)which I don't want to change.  Frankly I don't EVER want the program to ASSUME what I want to see in the tree, it should stay EXACTLY the way I left it until I change it.

The biggest difference is the difficulty of manuvering in a 3D environment in SW.  Example to draw anything in SW you need a plane to draw on at the EXACT point in 3D space you wish to draw.  In vellum planes are infinite.  If I have the front plane selected I can draw on the front plane anywhere on any part, or just out in random space (then move the part to the final location later).  Or, I can select a part then click on any point on a drawing and extend a line in the proper direction (it automatically snaps to axis & tangencies) to mirror a part.  Or transfer any dimension from any part to any other part without needing to measure it and make notes.

Consequentally, all the time spent creating planes, axis, worrying about origins, measuring existing parts, ect. is just wasted time due to software limitations (at least in my mind).  I'm used to it, I can work around it, but I find it incredibly tedious and slow.  I've lost the FUN in solid modeling (work is much more work then it used to be).

RE: History-vs-Non History based CAD softwares

A POSSESSED SLINKY!  HA!

I think many share your sentiments regarding the feature tree.  I'd like to be able to toggle off the tree action when selecting thing as an item on a toolbar instead of something burried in the Options.

I believe SW was set up the way it was for constrained engineering purposes, and less for quick form creation.  (That's why so many ID guys/gals like Rhino for doing so.)  However, coming from ACAD, where you have to specify and fully constrain everything just to draw a line, SW was quite a "loose" feeling tool in the engineering field when released.  Things could actually remain unconstrained indefinitely (albeit with the limits you discussed regarding plane placement, etc.).

Although I'm an industrial designer, I do my own plastic part engineering, etc. for production and leverage great utility from the history (having undergone the full mind "warp" to play nice with SW).  For quick form development without dimensional hindrance, a NURBS-based, push-pull-surface program would probably be of more use.  Past that, into the quantified and absolute sphere of engineering, SW sings.  And that's what it was designed to do.

Certainly, it pays to use the right tool for the job.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: History-vs-Non History based CAD softwares

You're right Theophilus.

I was a Pro/E user, back in those days where Pro/E only worked in UNIX workstations (last used version was V17).
For these versions there was nothing like unconstrained sketches. Everything needed to be 100% constrained. Every modification on the design, by changing sketch dimensions or feature dimensions, needed to be very whell planned because Pro/E could "easely" fail to rebuild (this is not a complaint; it was the state of the art at the time).

When I started to use SW, I was surprised how tolerante it was. No need for fully constrained sketches, almost all modifications could be successfuly performed, no matter how different the result was. So it sounds a little strange to hear someone complaning how rigid SW is!

As I told before, the type of work is the firts thing to analyse when deciding the type of CAD to use. The last post from ongybill prove this. I get the feeling that puting a ID guy using SW it will be like puting a painter painting using a drawing board and a ruler. But I can't imagine doing my work (that also includes ID into some extent) without a good history.

Regards

RE: History-vs-Non History based CAD softwares

I think I've confused people.

I'm not complaining that SW has a history tree.  I'm used to that.  But, that it ONLY has a history tree.  (Don't get that)

As far as solid model creation Vellum is superior (in my estimation).  There are a few advantages of SW 2005 over Vellum 2000, but from my research on Cobalt 2005 most or all of those advantages no longer exist.

Vellum is vastly superior to SW for 3D drawing (solid or sketching).  MUCH easier to move parts around, create parts, use references from existing parts, assembling parts, ect..  You can acurately draw very complex parts 100% 3D w/o ever making a single 2D sketch; drawing so much as a single line or point; defining a single plane or axis; inserting a dimension; ect..  SW doesn't even come close to this functionality.

Bottom line is SW is good software.  Not the best, but perhaps 2nd best (I'm too out of date to know).  It typically takes me 3-4 times as long to create 90% of the models I create w/ SW (this will reduce some w/ experience, but not that much).  The other 10% of models are quicker or equal w/ SW.  Most things w/ SW simply take more steps, more commands, & more mouse clicks to acheive the same results.  

The models once drawn have no appreciable benifits over each other.  Both are "smart" solids, both have a history tree, ect..

I'd rank them this way:

For 3D solid design I'd give Vellum a 9 and SW a 5.

For 3D solid drawing (drawing things that are already designed) I'd give Vellum a 8.5 and SW a 7.

For detail drawings I'd give Vellum a 6 and SW a 8.

For file management I'd give Vellum a 8 and SW a 4 (sorry assemblies with hundreds of part files still drive me insane, much prefer 1 file for 1 assembly).  

For finding pre-drawn parts on the web I'd give SW a 10 and Vellum a 1 (it's fringe software, no where near the # of users).

For modifying and using imported parts (something I do quite often) I'd give Vellum a 10 and SW a 2.  Vellum can easily use 3D wireframe data to create models, and can work with dumb solids w/ almost zero problems; neither is true for SW.

RE: History-vs-Non History based CAD softwares

Quote:

For 3D solid design I'd give Vellum a 9 and SW a 5.

For 3D solid drawing (drawing things that are already designed) I'd give Vellum a 8.5 and SW a 7.

For detail drawings I'd give Vellum a 6 and SW a 8.

For file management I'd give Vellum a 8 and SW a 4 (sorry assemblies with hundreds of part files still drive me insane, much prefer 1 file for 1 assembly).  

For finding pre-drawn parts on the web I'd give SW a 10 and Vellum a 1 (it's fringe software, no where near the # of users).

For modifying and using imported parts (something I do quite often) I'd give Vellum a 10 and SW a 2.  Vellum can easily use 3D wireframe data to create models, and can work with dumb solids w/ almost zero problems; neither is true for SW.

I want to see the models you are making your poll on. I bet I can out do Vellum in many different ways.

Break down:

Quote:

For 3D solid design I'd give Vellum a 9 and SW a 5.

Why? What are you modeling in Vellum that you can't do better in SW? - Please list a place where these files can be uploaded.

Quote:

For 3D solid drawing (drawing things that are already designed) I'd give Vellum a 8.5 and SW a 7.

I don't understand this? "(drawing things that are already designed)" You mean you can't make a drawing in SW better then you can in Vellum for models that are already in SW? Please elborate.

Quote:

For detail drawings I'd give Vellum a 6 and SW a 8.
Even though you gave SW a higher score, im still surprised, because SW draiwng usually get a low score, because they are not AutoCAD drawing, and most user frown at SW drawings. However I think they do a great job and always had since I started using them in 96 and at the point SW was limited versus where it is at now.

Quote:

For file management I'd give Vellum a 8 and SW a 4 (sorry assemblies with hundreds of part files still drive me insane, much prefer 1 file for 1 assembly).

File management does suck, but that what PDMworks is for. It is to help you control and track your files better.

I had system at one of my previous employments, without PDMworks and we setup a system that worked for us quite well and again that was in 96 when SW was extremely limited. I think if you had the proper tools you wouldn't feel the way you do about this.

Quote:

For finding pre-drawn parts on the web I'd give SW a 10 and Vellum a 1 (it's fringe software, no where near the # of users).

Of course and there is a reason for that... because SW is better then Vellum. If Vellum was that good then SW would be the one with limited models online.

Quote:

For modifying and using imported parts (something I do quite often) I'd give Vellum a 10 and SW a 2.  Vellum can easily use 3D wireframe data to create models, and can work with dumb solids w/ almost zero problems; neither is true for SW.

This varies depending on the Data translator the files came from. What type of files do you import into Vellum and SW? The "types" may be the problem, more then the import. Your Options maybe not be setup correctly or not set up efficiently. Please list the types and a site to what files you are importing. I would like to see this for myself.


Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: History-vs-Non History based CAD softwares

Ongybill, how long have you used Vellum and how long have you used SolidWorks?  I think you are experiencing "software familiarity" rather than "software limitations".

"I think there is a world market for maybe five computers."
Thomas Watson, chairman of IBM, 1943.
Have you read FAQ731-376 to make the best use of Eng-Tips Forums?

RE: History-vs-Non History based CAD softwares

Howdy,

Don't have a great deal of time at the moment.  

MadMango is certainly right that much of my frustration is a function of software familiarity.

My biggest annoyance with SW is the difficulty in 3D design work.  I confused scott some with this.

I break it down into solid drawing; where you pick up something measure and draw it, or you take a 2D drawing and draw a solid model using the dimensions on the drawing.  No design work required.  Then there's solid design, where you have to design parts from scratch.

Both programs are capable of this, but in SW's case, the software itself inhibits rather then helps the design process.  Being limited to drawing on fixed point planes makes it very time consuming and slow to attempt to transfer points from parts A & B to connecting bracket C you are attempting to design.  3D sketching capabilities in SW are pathetic.  Here I'd give Vellum a 10 and SW a 1, there is no comparison.  SW has other features that help later in the design process, thus I upped it's score to a 5 and lowered Vellum's to a 9.  But, for whipping up a quick sketch to work through several different design ideas SW sucks.

One thing I've found as I gain more design experience is that designs get more complicated because instead of struggling to think of something that'll work I have to quickly decide on one of the 6 different ideas that pop into my head.  It's quite easy to do this in vellum by simply positioning known parts in approximate locations and sketching ideas around them.  Using a combination of simple solid shapes and 3D wireframe.

With SW it's easier to sketch on paper (which I'm not that good at).<G>  An article I recently cut out of Design News (I think) says it better then I can: "CAD systems often constrain engineers rather then liberate them to do their best and most creative designs....Most CAD tools available are not focused on creativity...The tools are meant for documenting not creatively developing a design.  I find SW extremely constricting when designing things.  SW is very inferior when it comes to ease of manuvering and manipulating things in a 3D environment.

I'd disagree that market share means a product is 'better'.  For many years Apples OS was vastly superior to Windows (not much difference anymore).  Autocad was lousy software when I learned it, vastly inferior to CadKey which I also used, but it still dominated the CAD world for years (only meant it was more well known and marketed better, not that it was better).  Vellum made the mistake of being strictly Mac software, up until about 2000 which greatly limited their market.

I will say that I can, eventually, draw most anything I wish to with SW.  But, in many instances it's not nearly as straightforward as I'm used to, takes many more steps, and I spend the majority of my time not thinking about the design and how to improve it, but how to use the software (hopefully that'll improve).

RE: History-vs-Non History based CAD softwares

I'll have to investigate PDMworks.  Never used it.  Anything that'll help with file management would be welcome.

As far as imported parts, usually these are provided by customers (old Autocad files being most common).  Perhaps there's a way in SW to import 2D wireframe data and then use the 2D wireframes to create a 3D solid, but I had zero success when I tried.  My main comment was being able to take existing 2D files and converting them to 3D solids.  If there's a tutorial or someplace where I could get suggestions on how to do this in SW I'd love to know about it.  I could only import Solids, not wireframes.

{I want to see the models you are making your poll on. I bet I can out do Vellum in many different ways.}

You're probably right, I've seen, and learned from, your web-site, and you're obviously an expert w/ SW.  I think it's simply the time and # of steps to draw something that drives me nuts with SW.  I can draw pretty much anything I wish to with SW, it just takes more time and steps (creating planes, axis, 2D sketches, adding dimensions, ect that aren't necissary in Vellum).  Perhaps many of these steps can be eliminated with experience.  I hope so.

The only model I have anywhere on the web is http://www.3dcontentcentral.com/3dcontentcentral/cc_frame.asp  It's a part I drew in SW (limit switch roller). Not sure it's helpful at all.  Though it'll likely just show you what an amatuer I am with SW's.<G>

Anyway, gotta get back to work, thanks for your time.

Bill

RE: History-vs-Non History based CAD softwares

ongybill,
How much experience do you have with SolidWorks or any CAD software? And how much mechanical design experience? Not trying to trash you in any way, just trying to get an idea where you are in the way of comparing CAD software.
Also, if this discussion is to go further, there should be a new thread.
thanks

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site
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RE: History-vs-Non History based CAD softwares

I take items off my desk and design them every day. How do you think the Bionicle made it into SW?... not from dimensions given to me. http://www.scottjbaugh.com/Desktop%20images/Bionicle%20Image1.jpg

CBL posted this in another forum http://www.ashlar.com/sections/support/tutorials/modeling_process/modeling_process.pdf - and I can't express how easy this is to accomplish in SW and they seem to be completely Identical in function... I'm sure Vellum copied SW in that respect.

Under the "A" section of page 2 -  

Quote:

but it will take a bit of extra work to create the rounded end.

What are they talking about that is a drop in the bucket even for them most newest of users. If you have done the Online Tutorials then this should be easy!


Quote:

Both programs are capable of this, but in SW's case, the software itself inhibits rather then helps the design process.

Then why is SW leading the pack? I think a lot of your problem is that you are not experienced enough with SW to know the proper function or how to use the software correctly. Plus you probably can't let go of an older CAD system.

 

Quote:

Being limited to drawing on fixed point planes makes it very time consuming and slow to attempt to transfer points from parts A & B to connecting bracket C you are attempting to design.

Construction geometry and construction planes will fix this problem. If you know how to manipulate the planes this is easy to accomplish.

Quote:

3D sketching capabilities in SW are pathetic.
They have not been the best, but after years of working with them the are not that bad. You have to just understand how they work. SW06 is going to fix a lot of the 3D sketch limitations though.

Quote:

Here I'd give Vellum a 10 and SW a 1, there is no comparison.  SW has other features that help later in the design process, thus I upped it's score to a 5 and lowered Vellum's to a 9.  But, for whipping up a quick sketch to work through several different design ideas SW sucks.

Have you seen the bionicle? That mask was made with several 3D sketches, surfaces, etc... to get the correct shape. I want to see you make that shape/mask in Vellum. With it's "9" in 3D sketching.

Quote:

One thing I've found as I gain more design experience is that designs get more complicated because instead of struggling to think of something that'll work I have to quickly decide on one of the 6 different ideas that pop into my head.  It's quite easy to do this in vellum by simply positioning known parts in approximate locations and sketching ideas around them.  Using a combination of simple solid shapes and 3D wireframe.

just a couple things come to mind:
Configurations of parts
Assembly sketches

With assembly sketches you can then start a new part in the assembly and convert those sketches into parts and then you have your part in the assembly... How easy is that?

Quote:

With SW it's easier to sketch on paper (which I'm not that good at).<G>  An article I recently cut out of Design News (I think) says it better then I can: "CAD systems often constrain engineers rather then liberate them to do their best and most creative designs....Most CAD tools available are not focused on creativity...The tools are meant for documenting not creatively developing a design.  I find SW extremely constricting when designing things.  SW is very inferior when it comes to ease of manuvering and manipulating things in a 3D environment

This is because you don't know how to use the software. It's apparent in your answers. If you would use some of that negative feedback towards learning proper function and use in SW you would understand why we use the software everyday and why we don't use Vellum

Quote:

I'd disagree that market share means a product is 'better'.  For many years Apples OS was vastly superior to Windows (not much difference anymore).  Autocad was lousy software when I learned it, vastly inferior to CadKey which I also used, but it still dominated the CAD world for years (only meant it was more well known and marketed better, not that it was better).  Vellum made the mistake of being strictly Mac software, up until about 2000 which greatly limited their market.

Who ever said market share makes a better product? Function, function, function is the best CAD tool and SW provides it if you only understood SW. I now not only think your Biased towards SW, because your MAC guy and you are trying to convince us out here that MAC is the best. MAC's are good, but SW is a great application and just because they don't support MAC doesn't mean we should change to Vellum. If you only understood the application and proper use you wouldn't be posting such negative things about SW.

Quote:

I will say that I can, eventually, draw most anything I wish to with SW.  But, in many instances it's not nearly as straightforward as I'm used to, takes many more steps, and I spend the majority of my time not thinking about the design and how to improve it, but how to use the software (hopefully that'll improve).

It's not straight forward because your used to a certain way and your unwilling to give 100%. If you forgot completely about Vellum and truly tested SW to it's full potenial I think you would understand why we use it.

In conculsion:

Your knowledge of the SW Software is way too limited for you to be judging the software. You need someone like a VAR to train you on proper function and technic. Your Polls are miss leading because the files you are making are probably easy to make in SW, you just don't know the proper function to make this file SW. I still challenge you to make not only the Bionicle Mask like mine, but also to post some of your models from Vellum, that you think takes to long in SW to make or can't be made.

If you don't accept these challenges, then how can we honestly trust your opinion about Vellum, but that may just be my opinion.

Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: History-vs-Non History based CAD softwares

We're not communicating very well, so there's little point in continuing this.  For example I'm not a mac guy and wouldn't advise anyone to buy one today. Too many assumptions.

I do have lots of questions agout SW.  I'll occassionally post specific ones.

I don't believe I've ever said there's anything that's impossible to draw with SW.  Nor have I ever claimed to be an expert, not even in Vellum.  I do however use both programs every day side by side.  I see many things that are easier to do in Vellum.  Perhaps it's due to a lack of training in SW.  But more and more I think it's just that SW takes more commands and more effort to do certain things.  INCOMPREHENSIBLE AS IT IS.  Doesn't mean SW isn't good or even GREAT software, but that it's not the BEST AT EVERYTHING.

From my EXPERIENCE with both programs Vellum is MUCH easier to learn on your own.  Even though SW's tutorials are better then any I've used from Ashlar.  My OPINION.

END OF DISCUSSION

I'll post this as a seperate question, but just one thing that is much easier to do with Vellum.  I draw a LOT of electrical boxes.  So, I punch a lot of holes in boxes for connectors.  With Vellum I have a lot of connector models that also have 2 solid model hole patterns (1 for clearance & 1 for tapped holes).  With Vellum I insert the connector in the drawing with the box then simply put the appropriate hole pattern model where I want the connector & subtract it.  This instantly gives me all 5 holes properlly sized and placed.  Quick & easy.

Is there a good way to insert standard hole patterns in SW's?  I have dozens of standard connector sizes we use.  Really don't want to keep drawing 5 holes ea time I need a connector somewhere.  I know I can place the connector then use that to locate the holes, but still much slower.

I've been attempting to do something similar with SW.
Thought I could do it with the JOIN command, but that doesn't seem to work in assy mode, neither will the cavity command.  I can't insert the connector layout model into a part file and then subtract it.  If I draw the model IN the part file then I can subtract it, but it's easier to just draw a sketch and holes at that point, so what's the point.  Can't figure out any way to do this with hole wizard.

Ok, figured out how to do it.  IF I take the box model part, then create an assembly w/ the box in it, then insert the hole layout model into the assembly & position it, I can use the cavity command to create the holes.  Process: place part into assy, place hole parts in assy, pick the box, select edit part, then pick the cavity command, then select the hole model/s.  Then HIDE the hole model/s & the holes are there.  But, you cannot ever delete the hole models.  You can only hide them.

For a connector panel with 20 connectors on it, that means I have 20 extra models I have to keep.  Works, but not as easily, requires more steps, more models (3 models/connector not 1), and the end result isn't as clean.

Is there a better way to do this?  I haven't found it.

RE: History-vs-Non History based CAD softwares

Library Features will make it easy for you insert different connector cutouts.  I also design "black boxes" and use a mixture of mil spec and commerical connectors....I create the cutout once and store it as a library feature for use on another project...

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

Do you trust your intuition or go with the flow?

RE: History-vs-Non History based CAD softwares

My point is don't go judging both pieces if you don't have enough expereince in either of them. It's Obivisous you don't. So running Scores like Vellum 10/SW 1 - is BS, because you giving a negative image about something you know little about.

Sorry you have taken offense to this, but I don't think you should judging something you know nothing about.

I have not judged Vellum in a poll versus SW. I think SW can run circles around Vellum with just the few PDF files I have read recently. Vellum pushes out how great it is and the PDF tutorials and white papers are just ways of blowing steam up the you know where.

Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: History-vs-Non History based CAD softwares

I wonder how do you know if his comparison is inaccurate?  Have you ever used Vellum?  Let's not be too defensive!  Nothing is perfect.

I would agree that solidworks doesn't allow you to be nearly creative enough... having said that, I am getting used to it and it is still a productivity boost from anything else...

We just wish it had only good sides and no bad... well... tough luck I think!

RE: History-vs-Non History based CAD softwares

Well I've been out from this thread from sometime because I was feeling that it was turning into a discussion somewhat different from the original question.

But Pevac inspired me for a final statement.

For that I will use an example. Imagine that you by a good car: a Mercedes. You can enjoy this car and feel that it's the best car in the world. Now put it off road. Will it perform OK? NO. Why not, if it's a good car? Because it was not designed to do it. Thats why Mercedes have the ML jeep. So don't compare prices between these two to choose one. Otherwise you will end coursing your decision when you are stucked with your car in the middle of the sand, but don0t blame Mercedes.

SW is a mechanical design CAD. And it's a good one, competing in a very hard market and ganing a good positon. Is it creative? Yes, from the machanical design point of view. Could you perform better with other CAD? I am shure that ther are Pro/E users, or SE users that would not change to SW for "anything" on the world. Every CAD have their strengths and weeknesses. But I am also shure if the transition was needed, sunner or later this "other CAD" user would be performing very well on SW (I know it, I'm one), maybe doing things a bit different, but having good results.

But I am comparing products of the same family: mechanical design CAD.

So, the original question from btcoutermash it's triky, because he/she want's to benchmark a Mercedes car with a Mercedes Jeep. He/she either need a car or a jeep. So he/she should benchmark Mercedes car with other cars (BMW, Volvo,...) or Mercedes jeep with other jeeps. But first he/she need to know what type of vehicle suits him better.

And a final note. SW is improving it's tools for surface generation, being more suitable to use in industrial design.
Although I am concern primarely with the product functions rather than the product appearance, I also take care of this issue. And I can live happily with SW. But I see others like Ed Eaton or Theophilus (among others) or companies like DIMONTE or IDEO using SW for industrial design. Could they be that wrong?

Regards

RE: History-vs-Non History based CAD softwares

My only comment ... why isn't there a Vellum forum here?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site
FAQ371-376
FAQ559-1100

RE: History-vs-Non History based CAD softwares

gunnykiln (Mechanical)
As a Vellum user since 1996 and recently had to switch to SW I agree with ongybill in his comparison assessment. Moving from Vellum complete design freedom to SW extruded 2D sketches is a little like tying one arm behind your back when sculpting. Or playing pool and suddenly only being allowed to make bank shots. Sure you can still get it done, but its going to take longer and will feel awkward for a while. It's hard to explain to people that haven't used it, but in Vellum you design "the thing"  directly and intuitively where as in SW "the thing" is the cobbled together result of a list of sketches and features. It's oblique as opposed to direct.

While I am sure a lot of it is familiarity, the odd thing is, the more I learn SW the more my opinion is reinforced.

I do think the drawings (fabs) part of SW is vastly superior to Vellum's dimensioned drawing functions.

RE: History-vs-Non History based CAD softwares

The other evening I spent looking through the Vellum tutorials. What I saw was not what you & ongybill describe. I expected to see  a super-duper CAD program ... what I saw was 3D AutoCAD on steroids. I'm quite willing to accept that Vellum has some advantages over SW, or any other solid modelling program, but I did not see anything in these tutorials to prove that.

Basic Modelling Processes ... http://www.ashlar.com/sections/support/tutorials/modeling_process/modeling_process.pdf
Oh look ... 2D sketches being extruded.

Tutorials ... http://www.ashlar.com/sections/support/tutorials/tutorials.html
Create a Bill of Materials in Graphite & Create 2D Isometric Drawings ... these are jokes, right?
Create a Simple Bowl ... what is soooo different in how this would be created in SW?

If these tutorials are a true reflection of how to use Vellum, then you are welcome to it.


Making the best use of this Forum.  FAQ559-716
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Helpful SW websites every user should be aware of.  FAQ559-520

RE: History-vs-Non History based CAD softwares

Hey gunny,

I was beginning to think I was the only one here who'd ever used Vellum.  I'd used Vellum so long before SW, that I'd totally forgotten how difficult and convoluted CAD could be.

Reality I was totally sold on SW being vastly superior to Vellum before I used it, then amazed how difficult it actually was to use.  And how incredibly restricted designing in 3D is.  

{It's hard to explain to people that haven't used it, but in Vellum you design "the thing"  directly and intuitively where as in SW "the thing" is the cobbled together result of a list of sketches and features. It's oblique as opposed to direct.

While I am sure a lot of it is familiarity, the odd thing is, the more I learn SW the more my opinion is reinforced.}

Very well said, couldn't agree more.

As to the comment why isn't there a Vellum forum here.  It's so simple to use, why would there need to be.<G>  

Going to a forum and online tutorials to try and figure out how to do things is totally new to me with SW, with Vellum I could always figure it out on my own.

RE: History-vs-Non History based CAD softwares

That has been my point all long! You are still trying to make SW into Vellum. It's hard to forget your old CAD when you have move to a new CAD. I'm not saying SW is superior to all other CAD. I'm saying that what I have saw from CBL and your comments, isn't anything SW can't do and I think it can probably do it better. It's just that you don't know How to do it, because your mind is stuck in the Vellum world.

Every one I talk to think they have SW figured out. And that's not true. I am still learning new things everyday. THere isn't one person out there that can say they no the entire package. you only what you do and if you haven't had a vast amount of different things to do in SW, then you haven't used it to it's full potenial. If you would please provide me with what it is you guys are describing [i]like I keep asking for you too[/u] then how can I or anyone else understand your point about Vellum? Please if you have an example then post it. I want to see what takes longer to do in SW versus Vellum. I'm just asking you to prove this over telling me.., If either of you can show me a few examples other then describing and giving a poll, then please by all means do so.

ognybill,

if you don't have the terminology then you will not be able to find what you are looking for in the help or in SW.

Example:

SW - Uses Circular patterns
AutoCAD - refers to those as Arrays

Neither are the same terminiligy, but they mean the same. How would you look that up in the SW help, if all you ever knew was an Array?

Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: History-vs-Non History based CAD softwares

Hey Scott.  Sorry to keep wasting your time.

I can't forget Vellum, because I still use it everyday.  I'm constantly switching back and forth (which doesn't help my confusion level any, but has to be done).  In fact I find myself getting confused in both programs at times.

So far I haven't done well giving examples, but I'll try again.

Things that are easier:  (Most (maybe all) of these things can be done in SW, just harder w/ more steps).

Being able to modify any part of any assembly all at once (no need to go into edit part model and work on 1 at a time).  Say I want to put fillets on the corners of 10 different parts w/ 5 different radii.  This can be done as 1 command picking any edge on any part and modifying the radius at any point.  (I'll often add all the fillets after the basic fixture is designed, time to pretty it up).  This takes much more time in SW editing ea part seperately, and each different radii requiring a seperate command string.

Being able to grab any part at any reference point and drag it to any other reference point & attatch it, or hold down control and move copy.

Being able to draw with primative shapes (2 clicks creates a cylinder, 3 clicks creates a block, ect).

Being able to use any point or combination of points on existing parts or sketches to create solids, or as references.

Being able to use existing geometry to set move or move/copy distances.  

Being able to draw construction lines vertically or horizontally with a simple mouse drag (very useful for seeing how parts line up in an assembly.

Being able to draw things the right size as you draw them w/o ever having to add dimensions.  Each dimension requires 3 extra clicks, and I find the dimensions are often in the way & slow me down in 2 ways: 1 making it hard to see what I'm drawing; 2 dragging them out of the way or zooming in/out so I can see to select what I want.

Being able to pick a part/s then pick any point/s on any other part/s and drag a line to mirror or mirror copy those parts around.

Having the drafting assistant select intersections.  I know it's suppossed to, but seldom can I get SW to select an intersection, so I find myself trimming 1 line so there's an endpoint for it to grab.

Never needing to select a finite plane to draw on.  Example, being able to draw on the front surface/s of any and all parts at the same time.

Being able to draw all the details I want at the same time (not having to make several sketches).  Example I want to draw both pockets in and extrusions on the surface of a plate.  In SW I have to make a sketch to extrude, and another sketch to extrude cut.  In Vellum I can pick any combination of sketch entities to make a feature from.

Never needing to draw in centerlines or planes to mirror, rotate around, draw on, ect..

Being able to pick any face of a part, like a motor face, and extrude a new part from that face.

Being able to mold a solid object like playdo.  stretching, contracting, adding, subtracting, cutting it into pieces, scaling it, ect..

Never having to care how a model was assembled when you modify it.

Never having a model have rebuild errors because you deleted the feature that later features were referenced off of.

Having 16 undos instead of 1.

True 3D sketching (with circles, polygons, being able to extrude parts from 3D sketches, ect.)  Not many sketch tools work in 3D sketch.

True 3D drafting (not needing to start each part as a 2D sketch).

Being able to store lots of similar parts in one file then simply picking the one/s you want and copy pasting them into another drawing. (ie a file with 20 different weld connectors (not 20 files that each have to be opened seperately)).  Just ran into this, it takes me a lot longer to assemble common components into an assy because they're not in 10 files, but in 40.  It just takes longer to got through all the extra files and folders to get to the parts I want.

Being able to totally detatch a drawing so it never changes regaurdless if the models are changed.  Both for history and, so you can have a line drawing that you can modify just like a sheet of paper.  (Something I use a lot when I need to do a concept drawing for something similar to something we've built before.  With vellum I can take bits and pieces from several drawings, put them together, add a few lines & make them look like a complete system (more of an art function then an engineering one, but extremelly useful).

Being able to only have associativity if I want it.

Being able to take a model cut it up, take the piece of the whole I want, and discard the rest of it w/o any messing up previous assys using the whole part, or having rebuild errors.

Being able to use imported parts w/o errors.  Lots of parts I've imported from Vellum need to be redrawn because they are permanently flagged, don't draw correctly, or will only allow me to have 1 mate.

Being able to simply put a part where I want it w/o having to lock it down with 3 mates.

Being able to simply delete any part/feature that I want to without worrying about messing up something else.  Several times I've deleted part B that's mated to part A and suddenly I have mate errors with parts X, Y, & Z (don't think I'll ever understand why).  Same with parts where you have to suppress certain mates, then add mates, then unsuppress the 1st mates to have them work (just a bug, but an annoying one).

Being able to draw parts in context w/o problems.  Drew a nut on a stud in an assy 2 days ago.  It'd only let me have 1 mate no matter what I did.  Finally I deleted the part, reinserted it and it mated fine (yes I removed the inplace or incontext mates).

Not having the software crash on me so often (I'm using SP0 I'm sure that's part of the problem, but our head engineer won't let me upgrade).

Not having to click on a green checkmark 600 times a day.

Sorry, too long a list, and some of it's downright trivial.  What I miss most is the extreme ease of moving around in a 3D environment in Vellum.  If you've never experienced that it's hard to explain.  If I could regain some of that with SW the rest are minor things.  Vellum has a bunch of minor annoyances I just work around too.  No software's perfect.

I know I've come acrost too hard on SW when in reality there's a lot I like about it.  I also know that a lot of what I'm suffering from is a lack of training, but there's not much I can do about that.  I am finding 2 things with SW.  1) It'll do a lot of things I've been told it won't.  2) It's more user friendly then I gave it credit for.

Anyway, I have learned a lot from your posts & your website.  Thanks for the help, eventually I'll get it.  Gets a bit easier and more natural each day.

Geez what a rant, I'm embarrased.  Wordy even for me.

RE: History-vs-Non History based CAD softwares

I will put together a list ASAP of these things and see if I can't help you out. I will probably just post it to me site, because it would be probably 10x larger then this, because I will try and include Screen shots of it.

Maybe I can find time this weekend, but I'm not going to hold me breathe.

Best Regards - and thank you for the post!

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: History-vs-Non History based CAD softwares

To summarize some of my feelings on this whole discussion:

I think it all comes down to how comfortable you are with history-based, parametric modeling and how you are/are not using it.

History-based, parametric modeling can be an extremely powerful tool, but it can require much upfront planning an maintenence.  Some careful thought must go into all the dependancies and relationships that these types of modelers depend on.

Non-history-based, non-parametric modeling can be extremely flexible because you don't need to worry about all the dependancies and order of operations.  How you get there is irrelevent here.  Only the final representation has any meaning.

Both systems have their adavntages and disadvantages.  In many ways your arguments above mirror arguments between SWX and AutoCad (AutoCad beig a Non-history-based, non-parametric modeling tool).

RE: History-vs-Non History based CAD softwares

Scott, any help on any of those areas would be wonderful.

I think I've about tapped out the knowledge base here, and thanks to things like this forum I use lots of tools that I don't see anyone else using.

Arlin hit it on the head.  {I think it all comes down to how comfortable you are with history-based, parametric modeling and how you are/are not using it.}

Just hit me, I have 18 years CAD experience, but have never really used history based software before.  Vellum has it, and I use it now, but before starting SW I mostly ignored that functionality because I really didn't need it.

People have asked, so here goes.  Most of my experience is with Vellum.  I've also used CadKey, Master CAM (it's drawing functionality beat AutoCADS at the time so I drew some of my machining parts in the program rather then use AutoCAD, which was my only other choice at the time).

Tutored AutoCAD for a time, then didn't use it for a couple releases and couldn't draw the simplest parts when I tried again.  Found it was much easier to just sit down with CadKey and figure it out from scratch then relearn AutoCAD (hope I never use their software again).  Still remember going through their summary and learning that each new release had added, deleted, or, my personally favorite, changed what 2-300 commands did.

Also have used some programs that are on the ash heap now.  MatciCAD, MiniCAD, and a couple I can't even remember the name of, but those were 2D wireframe programs.  Things have certainly come a long way since then.

RE: History-vs-Non History based CAD softwares

Being able to modify any part of any assembly all at once (no need to go into edit part model and work on 1 at a time).  Say I want to put fillets on the corners of 10 different parts w/ 5 different radii.  This can be done as 1 command picking any edge on any part and modifying the radius at any point.  (I'll often add all the fillets after the basic fixture is designed, time to pretty it up).  This takes much more time in SW editing ea part seperately, and each different radii requiring a seperate command string.
I'm assuming that there is no assembly / part structure like Solidworks and that all parts are in one file? What happens when you want to use a part in several assemblies? Copy it? Does it stay linked?

Being able to draw with primative shapes (2 clicks creates a cylinder, 3 clicks creates a block, ect).
Might be able mimic something like this with library features. Create the cyclinder or box(sketch extrude) as a library feature then drag and drop from the library. Another way is to create a macro of the steps to sketch and extrude and assign it to a button to auto create these.

Being able to use any point or combination of points on existing parts or sketches to create solids, or as references.
Being able to use existing geometry to set move or move/copy distances.  

Not sure I completely understand these. You can extrude up to points and you can reference points in sketches. You can also use points to do point to point move/copy in a sketch. There are point to point mates though I don't recommned them as you'll need more mates to lock down a part.

Being able to draw construction lines vertically or horizontally with a simple mouse drag (very useful for seeing how parts line up in an assembly.
Create a sketch for reference and sketch lines, is this not the same?

Being able to draw things the right size as you draw them w/o ever having to add dimensions.
Not dimensioning a sketch is a sure way to mess it up later when a parent reference change. But with that said, you can type in value for sketch geometry. Sketch a line and type in the length.

Being able to pick a part/s then pick any point/s on any other part/s and drag a line to mirror or mirror copy those parts around.
In sketches, mirror around a selected line. Part and assy needs a datum plane. I'm assuming once you mirror this in Vellum, you don't have associativity?

Having the drafting assistant select intersections.  I know it's suppossed to, but seldom can I get SW to select an intersection, so I find myself trimming 1 line so there's an endpoint for it to grab.
Not sure on this, will the intersection option in quick snaps work? Need to see what you're attempting.

Never needing to select a finite plane to draw on.  Example, being able to draw on the front surface/s of any and all parts at the same time.
You can select a parts face to sketch on, is this not the same? What do you mean at the same time.

Being able to draw all the details I want at the same time (not having to make several sketches).  Example I want to draw both pockets in and extrusions on the surface of a plate.  In SW I have to make a sketch to extrude, and another sketch to extrude cut.  In Vellum I can pick any combination of sketch entities to make a feature from.
Try "contour select on the right-click menu. You can use one sketch for multiple features.

Never needing to draw in centerlines or planes to mirror, rotate around, draw on, ect..
Is it associative?

Being able to pick any face of a part, like a motor face, and extrude a new part from that face.
That would be useful. Believe it or not, you can do this in the loft feature, just no where else. I would suggest assigning a hotkey to "Insert Sketch" and the "Convert Entites" tools. Then you can quickly insert a sketch on a face, select the face and convert entities which will convert the faces edges to sketch geometry. Extrude from that.

Being able to mold a solid object like playdo.  stretching, contracting, adding, subtracting, cutting it into pieces, scaling it, ect..
There are some tools for stretching, twisting, (Flex). Solidworks really isn't intended to create geometry like this.

Never having to care how a model was assembled when you modify it.
Never having a model have rebuild errors because you deleted the feature that later features were referenced off of.

Once again, I'm assuming there is no associativity to maintain, otherwise I don't see how this is possible.

Being able to store lots of similar parts in one file then simply picking the one/s you want and copy pasting them into another drawing. (ie a file with 20 different weld connectors (not 20 files that each have to be opened seperately)).  Just ran into this, it takes me a lot longer to assemble common components into an assy because they're not in 10 files, but in 40.  It just takes longer to got through all the extra files and folders to get to the parts I want.
Maybe configurations can help here. You can create configs in a part file or assy file and vary dimensions per config thus creating many similar parts in one file. Drag it into an assembly and select the config to show. Works for drawings too.

Being able to totally detatch a drawing so it never changes regaurdless if the models are changed.  Both for history and, so you can have a line drawing that you can modify just like a sheet of paper.  (Something I use a lot when I need to do a concept drawing for something similar to something we've built before.  With vellum I can take bits and pieces from several drawings, put them together, add a few lines & make them look like a complete system (more of an art function then an engineering one, but extremelly useful).
Save as dwg and reopen it is the only option here. You could use the Solidworks explorer tool to copy an assy and all parts to play around with for concepts.

Being able to only have associativity if I want it.
Yes, Solidworks is built around associativity.

Being able to take a model cut it up, take the piece of the whole I want, and discard the rest of it w/o any messing up previous assys using the whole part, or having rebuild errors.
Again, I'm assuming no associativity.

Being able to use imported parts w/o errors.  Lots of parts I've imported from Vellum need to be redrawn because they are permanently flagged, don't draw correctly, or will only allow me to have 1 mate.
Import diagnosis should help to fix problems like these.


Being able to simply put a part where I want it w/o having to lock it down with 3 mates.
Is mating so bad? There is an option in the mate dialogue to use for positioning only which won't create the mates. I don't recommend it as it's easy to click drag a part out of position by accident.


You are used to modeling in a non associative world where sketching and positioning parts must be done precisely to start. More simlar to Autocad, in fact most new ex-Acad users complain about the same issues at first. As master Yoda says "You must unlearn what you have learned, then, only then will you see the true power of the sworks". On the flip side we've had users that learn CAD on Solidworks or some other parametric modeler and complain that Autocad makes them have to draw precisely and doesn't work well. I think the hardest concept of Solidworks to grasp though is the assy / part file relationships. Solidworks could take steps to make that easier to manage.

Ultimately, I guess it dpends on what you're modeling. Programs like Alias, Rhino, and 3d studio model without much care for associatvity because feature history isn't important and can slow you down, just gettting the end result is all that matters. Feature history and parametrics to me is important. Sometimes it can get in the way, just like in some cases where you don't have it, having it might be nice. Depends on what you do, how often you change stuff, and what changes.

Can you provide any pics or a website of the product you work on? Be helpful to see so as to provide suggestions in Solidworks. Not having fully associative parts and assemblies doesn't make much since to me. You don't have have design intent built in for when you make changes. For example, I may want a hole 2" from the edge of a plate no matter how long the plate is. Without creating relationships, modifying the length of the plate may mean that the hole doesn't move to where it should. another thing to modify and keep track of.

anyway, good luck




Jason Capriotti
Smith & Nephew, Inc.

RE: History-vs-Non History based CAD softwares

Wow Jason,

Thanks for a great post.  Don't have time to respond to much of it right now.  You're right that a lot of my 'issues' revolve around associativity.  I think associativity is great, some of the time.  Most of the time I find it a detriment to design and creativity.

I build custom equipment.  Lots of things that're similar, but not the same as anything else I've built.  So having part A be associative just causes me problems when I create a new design that uses part A modified.  Unless I'm really careful about how I save Part A before I modifiy it I mess up all my earlier work.  In Vellum I 'flatten view' on all detail drawings.  This totally disassociates them from the solid model and they're just 2D drawings, so I NEVER accidentally mess up a detail drawing for an older system when I change something.  Haven't found a way to do this is SW, so I save the final drawings as pdf files, just to be safe.

In short, I like associativity, find it very useful at times, but only when I can turn it off and on.  I'd rather not have it at all then be forced to have it all the time.

Couple quick responses:

{Being able to draw construction lines vertically or horizontally with a simple mouse drag (very useful for seeing how parts line up in an assembly.
Create a sketch for reference and sketch lines, is this not the same?}

Yes, but we were talking about speed.  Vellum hold down mouse button & drag narrow window (construction line appears).  SW pick plane, pick sketch, pick line tool, click 2 points, click on construction geometry.  Also in SW it's a seperate sketch in the design tree, and there's no command to delete all construction lines at once.  Certainly doable in SW (more steps, more time).  Just something I miss, but not a major thing.

{Being able to store lots of similar parts in one file then simply picking the one/s you want and copy pasting them into another drawing. (ie a file with 20 different weld connectors (not 20 files that each have to be opened seperately)).

Configurations will help on some parts.  I'm more talking about having say 40 gas fittings in one file.  Open file look at fittings select the ones you want & cut & paste into assy.  Parts are similar in catagory, not shape.

{Never needing to select a finite plane to draw on.  Example, being able to draw on the front surface/s of any and all parts at the same time.
You can select a parts face to sketch on, is this not the same? What do you mean at the same time.}

Here is the crux of the difference.  In most cases SW seems to force you to work on 1 thing at a time.  Edit 1 part, with 1 sketch, on 1 face.  Ect..

What I mean here is working on all parts in an assembly at the same time.  I'm used to simultaneously modifying several things at once.  So I pick the circle command once and draw in 40 circles, 10 different sizes, on 8 faces, of 4 different parts, all as one command.  Then later use them to add features.  Or pick offset lines and draw dozens of offset lines on several parts w/ one command string.

{Try "contour select on the right-click menu. You can use one sketch for multiple features.}

I'll try that again.  Tried to figure out what it did once w/ no success.  I'll have to spend more effort, as I'd love to cut down the # of sketches I have to create.

I just posted a few picts of some systems we've built.  I also took a couple snapshots of similar parts files so you'll see what I mean.

http://img38.imageshack.us/gal.php?a=1

RE: History-vs-Non History based CAD softwares

ongybill,
Can not open your pic link.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site
FAQ371-376
FAQ559-1100

RE: History-vs-Non History based CAD softwares

SBaugh (Mechanical)
http://www.scottjbaugh.com/Images/Vellum_vs_SW_-_ what_I_can't_do.doc

My reponse
Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: History-vs-Non History based CAD softwares

Very well done Scott!

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site
FAQ371-376
FAQ559-1100

RE: History-vs-Non History based CAD softwares

Jason 123 (Mechanical)
I build custom equipment.  Lots of things that're similar, but not the same as anything else I've built.  So having part A be associative just causes me problems when I create a new design that uses part A modified.  Unless I'm really careful about how I save Part A before I modifiy it I mess up all my earlier work.  In Vellum I 'flatten view' on all detail drawings.  This totally disassociates them from the solid model and they're just 2D drawings, so I NEVER accidentally mess up a detail drawing for an older system when I change something.  Haven't found a way to do this is SW, so I save the final drawings as pdf files, just to be safe.

New designs based off an old one should be all new files. You can use Solidworks explorer to copy them and rename them at the same time. I would ignore library parts (see below) though and leave them linked to the library.

As for the old project files, they remain untouched and left in the state that you left them in. PDF backups are still a good practise though.


Couple quick responses:
Yes, but we were talking about speed.  Vellum hold down mouse button & drag narrow window (construction line appears).  SW pick plane, pick sketch, pick line tool, click 2 points, click on construction geometry.  Also in SW it's a seperate sketch in the design tree, and there's no command to delete all construction lines at once.


What about the window select (draws a box), doesn't leave anything on the screen though after you release the mouse button.

Configurations will help on some parts.  I'm more talking about having say 40 gas fittings in one file.  Open file look at fittings select the ones you want & cut & paste into assy.  Parts are similar in catagory, not shape.

This sounds like standard library parts in which case using the library (task pane) would be the way to go. Parts that do size similarly could store in one file or they could all be separate. The files are stored in a central library and all assemblies would reference them. The task pane library sorts and stores these items in folders (Gas Fittings) (Screws) etc. Then you just drag and drop from the library into the assembly. YOu can add mate references too so that they "pop" into place and add mates automatically.



Here is the crux of the difference.  In most cases SW seems to force you to work on 1 thing at a time.  Edit 1 part, with 1 sketch, on 1 face.  Ect..

What I mean here is working on all parts in an assembly at the same time.  I'm used to simultaneously modifying several things at once.  So I pick the circle command once and draw in 40 circles, 10 different sizes, on 8 faces, of 4 different parts, all as one command.  Then later use them to add features.  Or pick offset lines and draw dozens of offset lines on several parts w/ one command string.


Lack of assembly structure and associativity seems to allow this in Vellum. You can't really build design intent into the model it appears, at least not like Solidworks does. You just model "dumb" geometry in space. I guess it depends on your needs, for the one offs design you are doing, perhaps Vellum is a better choice. Sounds difficult to me from a design perspective not using relations and mates and fully locking down all geometry so that it responds to changes the way I expect it.


I just posted a few picts of some systems we've built.  I also took a couple snapshots of similar parts files so you'll see what I mean.

Link didn't work

Jason Capriotti
Smith & Nephew, Inc.

RE: History-vs-Non History based CAD softwares

I'm reading this Tutorial http://www.ashlar-vellum.com/sections/support/tutorials/2d_iso_drawings/2D_Iso_Drawings.pdf on Ashlar Vellum.

Vellum doesn't use planes and 2Dsketches at all. They are building entire models from an Isometric standpoint, from the get go. I see why they are struggling with SW. The example in the tutorial can be made in SW in 2 sketches and 2 features, where as Vellum took way long to build a most simple part. If Vellum takes that long to build a simple part like that, no wonder you guys are struggling with SW.

When you sit down to use SW you are not thinking about how to accomplish this in SW correctly your still thinking Vellums way.

The example in this tutorial, can be made in 2 features. The first feature is a single 2D profile with Chamfer and notch in it and extrude it to a depth. 2nd feature will be too cut the ellipise in the side of the part.

You can change the location of the notch with dimensions, if you use Equations you could automate it further.

With Vellum you have to 1) window Select everything, 2) Drag it to location, 3) grap points to get the final position of the notch. To add the Chamfer you have to ctrl window select 2 points and drag to location. Drawing assitanct helps with this, where SW doesn't have a drawing assitance. SW gives the ability to the user to be in control.

With SW you can do this by changing 2, maybe 1 dimension if you have the parametric diemensions setup correctly. The Chamfer was added in the beginning, by changing the dimension you can control the angle.

Ellipse tool in Vellum requires 3 points and SW also requires 3 points. Center, height, and width. Dragging the points changes the size. Dimensioning the center with 2 Dimensions will control location.

Looking at this further reminds me of the Old CAD system we had back in College. It reminds me of the old command Projection, and other commands similar to that. I'm sure it has it's strengths, but I quesiton everything I have read in these Tutorials. I bet there are a number of key strokes you make without thinking about anymore and those will contribute to more time doing those operations. I say that because I keep seeing press this, press that.

Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: History-vs-Non History based CAD softwares

Scott, Actually in vellum you could easily create that model in about 30 seconds. It looks like a lot of steps in the tutorial because they show everything being done a certain way. You could more easily create the model with the rectangle tool than with the line tool that they use in the tutorial. Also, I believe the demo is for Vellum's 3D wireframe program not the solids program in which you would use different 3D tools and still create the model very easily without creating a 2D single sketch.

Vellum certainly has its weak spots, but its definitely not the ease and speed of creating things.

RE: History-vs-Non History based CAD softwares

Scott.

Thanks for the lengthy response.  I skimmed through it and it looks excellent.  I just copied and pasted it into a Microsoft Word file.  I'll see what I can learn from it and respond later in the week when I hopefully have more time.  Then I'll email the response to you at your web-site.  Just skimming through I saw a couple good suggestions.  Thanks again.  I really appreciate you sharing your knowledge of SW like you have.  It's helped more then you know.

Oh, the tutorial you linked to is for their 2D drafting program (Graphite).  So you're absolutely right that it's like the old CAD systems.  You're literally drawing an Isometric drawing that looks 3D, but isn't.  Much as you would on a drafting table.

Graphite doesn't compare in any way to SW; or Ashlar's Solid modeling programs.

There're other ways, but I'd most likely draw that particular part the same way in SW and Vellum.  With a single 2D sketch and an extrusion.

RE: History-vs-Non History based CAD softwares

Although I haven't read of any productivity comparisons for history vs non-history-based MCAD programs, Joe Greco (Mr. 3D) did write an article in which he picked the best program (with runnerup) for each of many categories. I will post the month and year of the Cadalyst issue that contained this "awards" article.

 Essentially, the Conceptual Modeling award went to IronCAD, which is a non history-based program. IronCAD also won the "Visualization" award for its ease of creating photo-realistic images. If any of you have used this program, you'd know why Joe Greco chose it over all the others. First off, it has catalogs of dozens of solid and hollow shapes that you simply drag into a scene. This alone often saves a nice chunk of time. The other nice thing about IC is that each shape, whether solid or hollow (negative) contains pull handles that allow you to (in real time) change the size of the shape in all (xyz) directions. While this is happening, the dimensions (which are there by default if you wish) are displayed and are changing in real time.

 In addition, the IC TriBall can be attached to any feature to move, copy, mirror, etc. This feature alone is worth the price of the software.

  I use both IronCAD and Solidworks and it is obvious to me that unless SW makes major changes to its core structure, it will never be as easy to use as a conceptual tool as non-history-based programs. Certainly, it is a very powerful program. However, "fun to use for conceptual modeling" is not a description I would bestow upon it any time soon.

  

RE: History-vs-Non History based CAD softwares

Quote (Shifter):

I use both IronCAD and Solidworks and it is obvious to me that unless SW makes major changes to its core structure, it will never be as easy to use as a conceptual tool as non-history-based programs. Certainly, it is a very powerful program. However, "fun to use for conceptual modeling" is not a description I would bestow upon it any time soon.

In the entire design process from conceptual to releasing mechanical drawings no one MCAD package is superior.  I think this link has proved this but I don't think SWx would have the user base if it didn't compete at a high level throughout the entire design process.  I think this link has been flogged like a dead horse....lets move on.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
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