History-vs-Non History based CAD softwares 8

[btcoutermash]

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

 

[engAlright]

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

 

[macPT]

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

 

[MadMango]

History= feature driven models
Non-history= no features

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
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[Heckler]

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
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XP Pro SP2.0
NIVIDA Quadro FX 1400
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[ctopher]

Heckler, well done!

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
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[Theophilus]

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

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[CorBlimeyLimey]

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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[DesignSmith]

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

http://www.DesignSmith-Services.com

 

[macPT]

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

 

[Theophilus]

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

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[CorBlimeyLimey]

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.

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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[Heckler]

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

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?

 

[ongybill]

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.

 

[CorBlimeyLimey]

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.

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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[ongybill]

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.

 

[Theophilus]

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

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[CorBlimeyLimey]

ongybill ... good points & good examples.


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[CorBlimeyLimey]

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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[MElam]

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 . . .