Pro/E user attempting switch to UGNX
Pro/E user attempting switch to UGNX
(OP)
After over 10 years as a designer and CAD admin for Pro/Engineer I need to learn UGNX 4. This is proving to be quite difficult. I'm sure I'll have more questions but I'll start with this one. I have a cylinder 10" in diameter, 8" long and want to create a turned down section 4" in diameter and 5" down the axis.
I want to revolve a rectangular section about the axis of the cylinder to create in Pro/E terms, a revolved cut. I can seem to get the rectangular section created in UG sketcher but now I'd like to apply a diameter dimension in my sketch (4") to what would be the OD of the revolved cut. In Pro/E sketcher I would just drop a centerline down the center of the part, align it to the existing cylinder axis then dimension the revolved cut by selecting the sketch line, centerline, and then the sketch line again. Viola, I have a diameter dimension. How do I accomplish a similar scheme in UG?
Next I would like to constrain the other section line to the projected edge of the main cylinder OD and then constrain the bottom edge of the sketch to the lower edge of the large cylinder. In the end I want two dimensions driving this cut, the 4" diameter and the 5" cut length.
How do I go about doing this in UG?
Thanks...
I want to revolve a rectangular section about the axis of the cylinder to create in Pro/E terms, a revolved cut. I can seem to get the rectangular section created in UG sketcher but now I'd like to apply a diameter dimension in my sketch (4") to what would be the OD of the revolved cut. In Pro/E sketcher I would just drop a centerline down the center of the part, align it to the existing cylinder axis then dimension the revolved cut by selecting the sketch line, centerline, and then the sketch line again. Viola, I have a diameter dimension. How do I accomplish a similar scheme in UG?
Next I would like to constrain the other section line to the projected edge of the main cylinder OD and then constrain the bottom edge of the sketch to the lower edge of the large cylinder. In the end I want two dimensions driving this cut, the 4" diameter and the 5" cut length.
How do I go about doing this in UG?
Thanks...
--
Fighter Pilot
Manufacturing Engineer





RE: Pro/E user attempting switch to UGNX
You dont. Diameters, for the most part, simply do not exist in UG. You can't specify them, you cant measure them, its a mess. If you need to, you can dimension the radius from the center to the edge, and type 4.000/2 as the dimension. Unlike proe any expressions you enter will be retained (where proe solves the expression and stores the value only).
You might want to try drawing two concentric circles on the same plane, 10" and 4" diameters. Extrude the large one 8" long. Extrude the small one with a start value of 5, end 10, a two-sided offset of 0, 3, and a boolean subract. Just another way of looking at it.
I switched jobs about four months ago after using Proe 2001 for 8 years, now I use NX5.0.2 and am loving it. Interpart modeling is in the stone ages compared to proe, but direct modeling and all the flexibility are great. I hardly use any sketches anymore, I find the UG sketcher quite cumbersome though its hard to pin down why.
RE: Pro/E user attempting switch to UGNX
Therefore I create a 10" dia x 8" long cylinder as a primitive and created the 'Turned-Down' section with a subtracted revolved feature using an embedded sketch. To make it easy to edit the size of the 'Turned-Down' section, just open the file attached below and go to the Part Navigator, expand the 'User Expressions' item and now you can edit the "two dimensions" of the 'Turned-Down' section.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
You'll have to create isocline curves before the sketch feature, or, in the case of a simple cylinder, you can 'project' the face edges of the cylinder and make some reference entities using the quadrant points, and then align to the reference entities.
RE: Pro/E user attempting switch to UGNX
As for the 'diameter' dimension issue, anyone who thinks that it's hard work to use the expression system to create a diameter expression that is used to drive the sketch dimension via a math relationship is just looking for stuff to complain about.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
The issue with having to use "Radius=Diameter/2" is that you can't edit the diameter without going into the expression editor.
Specialty Engineered Automation (SEA)
http://www.sea4ug.com
a UGS Foundation Partner
RE: Pro/E user attempting switch to UGNX
RE: Pro/E user attempting switch to UGNX
You could use a primitive with bosses and grooves to define a turned part just as easily as you might sketch it.
Or you could just create a sketch with mirrored elements about the centerline that allow you to dimension across the diameter. I achieved the whole model in one feature for what it is worth.
Best Regards
Hudson
RE: Pro/E user attempting switch to UGNX
When I constructed models in Pro/E the mindset I had when creating them is "will I need to turn this feature off" So keeping in that way of thinking I constructed them in ways I knew would allow that. Hence my reason for not creating my revolved section like hudson888 did. There is no way for me to turn off the turned down section. Now the way JohnRBaker contstructed the model probably lends itself to supressing the turned down section if I needed to. I'll eventually figure out how to do that in UG.
Now, let me talk about the dimensions specifically. Again, I constructed models with dimensions I knew I was going to tolerance in the model and then SHOW in the drawing. I have seen many "glassy eyes" around here when I mention "why can't I just show my model dimensions?" So when I dimension a diameter in my sketech and tolerance it in my model I know thats what I will see in the drawing. If I want to flex my model dimensions in an assy tolerance stackup which was available in the assy mode of Pro/E I can do so by just flexing the diameter dimension.
Lastly, if my drawing represents what I actually modeled in the drawing I don't need to worry about someone coming along and detailing my drawing and possibly dimensionsing a feature from other surfaces that might not represent what I intended in my model. This is what really floored me about UG. You create your model and then you have to create a drawing by adding new dimensions. Well I my former world, the dimensions and design intent was already in the model.
Maybe NXMold and JohnRBaker could give some comments about my topics above. I'm not opposed to learning UG, I just need to understand some of the whys.
Thanks...
--
Fighter Pilot
Manufacturing Engineer
RE: Pro/E user attempting switch to UGNX
Another note, you've probably already found that you cannot create centerlines or mirrored constraints in sketcher, but the system can when you mirror geometry. That one blows me away. So you could take Johns model, mirror the inside edge of the rectangle, make it a reference line, and add your diameter dimension. Thats probably impractical for the most part though.
RE: Pro/E user attempting switch to UGNX
One more comment...
I've been using NX for two years now after 14 years with Pro/E and I have *maybe* reached 50% of the productivity I had.
My job involves making essentially the same parts over and over again with many small changes, so a parametric approach has proven to be the fastest. We do not use any primitives or direct modeling with NX - we start and end every model with 100% sketch-based design.
You *can* use NX in about the same way that you used Pro, but you will spend more time in your sketches. We stubbornly insist on 100% trimming and constraining every sketch even though the system does not require it. We do it because we feel that it conveys design intent better than untrimmed sketches.
My point is that if you try to use NX as an exact Pro/E replacement, you will experience some frustration. You have to decide whether to use all the modeling techniques NX offers and make your life easier, or stick with what you know and force the system to be used in a way that it can handle, but not as smoothly as Pro did.
There are tools in NX to accomplish whatever you want, but you'll have to depart from the Pro/E scripted way of doing things.
RE: Pro/E user attempting switch to UGNX
Pardon my ignorance, but what do you mean by "trimming" sketches?
RE: Pro/E user attempting switch to UGNX
I believe acciardi means close off your sketches. Good sketch practice, as I was taught, always closed sketches. We aligned to existing edges when we needed to and essentially always told the system "cut out this specific area or make this specific extrusion"
--
Fighter Pilot
Manufacturing Engineer
RE: Pro/E user attempting switch to UGNX
If you look at my example part attached to my original post, you will note that you can edit both parameters of the 'turned-down section' from the Part Navigator, without ever having to open either the sketch task or the expression system.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
The reference to not trimming a sketch might refer to the technique which we call 'select intent' where irrespective of whether the sketch curves were fully trimmed or not, the user is able to explicitly define which sections of the sketch profile, including defining what I guess you call 'virtual' trims on-the-fly, when using a sketch when creating a solid or sheet body feature. This allows several things including not having to waste as much time in the sketching getting every single curve trimmed-up so that there is only one single unambiguous 'loop', which often takes most of the time. Also it allows for the creation of filleted corners while still constraining them to the theoretical sharp corners of the an un-filleted profile without having to either trim the curve to the fillets and thus needed to add additional reference curves that need to then be constrained and dimensioned.
Note that this 'selection intent' approach is something that was adopted from Ideas that had something called 'hay-stacking' which did the same thing. Once you know how it works, you can save yourself a lot of what some people call drudge work when putting those last touches on a complex sketch.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
RE: Pro/E user attempting switch to UGNX
Yeah, I'm kind of anal about the whole design intent thing, so that's exactly what I do - mirror the whole sketch about the revolve axis.
Ed
RE: Pro/E user attempting switch to UGNX
Cheers
Hudson
RE: Pro/E user attempting switch to UGNX
I guess you're referring to User Expressions ?
And if a user expression wasn't used ?
Specialty Engineered Automation (SEA)
http://www.sea4ug.com
a UGS Foundation Partner
RE: Pro/E user attempting switch to UGNX
Diameter=10
p2=Diameter
'Diameter' shows up in the list of User Expressions while 'p2' does not. This way the user can control which parameters are exposed the world and which are not.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
Over the years, the sketcher has improved beyond all recognition, so that now it is a super tool to use, especially when sketches are linked within and across components.
There are several companies I have worked for that use sketches to the exclusion of everything else, so if you want a boss – create a sketch, fully constrain it , add dimensions, extrude, do the Boolean, and add blends, tapers separately - very time consuming.
With the example attached to the original post, using a cylinder, boss and hole, or a cylinder, groove and hole, I can create the model in a tenth of the time by this method rather than the sketch route. And all of these features use diameters and not radii in their definition.
Don’t get me wrong, the sketcher is the tool of choice on many occasions, but not always. Most of the time getting up to speed on UG is finding the right technique or method most suitable for the task in hand, and developing the foresight to predict downstream problems in choosing a particular method to model the component.
What are the thoughts of others in this forum?
RE: Pro/E user attempting switch to UGNX
Also any of you who can, should consider attending the UGS Connection Americas 2008 Users Conference in Orlando in June ( http://event.plmworld.org/index_2008.php ) as you'll get a chance to see more NX 6 than you ever imagined could be there
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
--
Fighter Pilot
Manufacturing Engineer
RE: Pro/E user attempting switch to UGNX
http://w
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
Looks interesting.....
Any clues?
RE: Pro/E user attempting switch to UGNX
But you have to understand people's frustration with change. While change may be good, it's also very difficult when you're forced to do it after so long. Not being able to make a diameter dimension is still one of my biggest peeves (along with not being able to reference existing edges or surfaces in a sketch).
To appreciate my frustration though, I think it depends alot on what you are designing. I've designed plastic bottles for the last 15 years or so. Picture a Downy bottle, or any of Bath & Body Works' funky shapes. I used the diameter dimension all the time for the width and thickness of the bottles. I also used those dimensions on the drawings. In fact, most dimensions on the drawing came from part sketches. To me, creating the dimensions over again was missing the point.
I should also say that I received virtually no training when I started working in NX. The company I worked for then had to save the money. Besides, how hard could it be? I already knew a 3d package? [heavy sarcasm] So I don't know the difference between direct modeling and interpart modeling. Because I creating everything in Pro as a wireframe first, then surfaced it and made it a solid (unless it was a round bottle), I sketched just about everything. So naturally, because I'm now doing the same work in NX, I'm still sketching all the time. It's the only way I know. I was shocked when I found some of the things that I couldn't do anymore now that I was working in NX. I'm sure someone just transitioning to ProE would think the same thing.
Like I said, I'm not trying to bash UG. I'd never get my questions answered if I did. [insert rimshot here] People like John, or someone who's been using UG for a long time and are very deep into it, probably don't take too well to criticism. I know I don't. Even constructive criticism. But before you denegrate someone who's used to using another system for so long and is stuck in a particular mindset, just accept that some people take well to change and some people don't. It should be obvious that I don't.
I hope I didn't offend anyone. That wasn't my intent. Someone asked for opinions. This is mine.
Mike
RE: Pro/E user attempting switch to UGNX
Any clues?
Join the Webcast on the 22nd and see for yourself
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
To Crocostimpy: I'm not a heavy sketch user myself, but I'm pretty sure there is a setting so that your sketch dimensions show up on the drawing (and I think you can even change dims on the drawing and have them propagate back to the model - but I'm out of my element here).
(emphasis mine)Sounds like even the long time UG users will be in the 'relearn' mode in the near future. But any product that claims to speed up design by 100x (excuse me, up to 100x) and I am a bit skeptical. How do you even measure a speed increase in the design cycle? Does a team do the same project twice and you see how much faster it is the second time? I would hope they speed up, since they have already worked out the end result. Do 2 different teams work on the same project? Different teams will come up with different designs in different amounts of time. Does the same team do 2 different projects? I think there are problems there as well. But I digress, the company I work for has a marketing department too. Wild, unverifiable claims either work wonders or backfire horribly. At least they have themselves covered with the "up to" in the fine print.
RE: Pro/E user attempting switch to UGNX
Chill!
I too see and feel the frustration of and with other users who think along the lines of their first CAD system. I've expressed that in the past and will like you probably continue to stand for fighting the good fight over the lowest common denominator that is ignorance. In the meantime I'll tell you about an interesting experience that I had last week.
I have recently had to learn another CAD system for work that I had slight knowledge of in the past and in doing so have come to realize how others view NX coming from the opposite experience. Not only do I now know what it is that they fail to appreciate, but I can also see how NX has in part mirrored other systems perhaps in order to better compete.
When I did this training I went in with my eyes open and expected to be called upon to rethink my ways of doing things. The truth is that NX is such a broad ranging and flexible tool that it was easy for me to grasp what has been presented to me, though occasionally difficult to deal with the limitations of both the system and my knowledge of it. Some of the functions are good. Some things that NX may have adopted they were right to do so. There are even a few things that NX is lacking and could improve upon.
However there is no direct modeling and no feature based modeling so the whole hybrid modeling word of flexibility is closed off to most other CAD systems.
I have been privileged to look into an alternative parallel universe that is this other system, (which I don't wish to name because this isn't about bragging rights or alienating other systems' users). I can even see how in a different reality it is possible to get by in a layer-less world, (if and only if you have the tools to manage it).
But hey NX is a hybrid system; Uni-graphics they used to call it. I always took that to have connotations alluding to the grand unified theory of CAD, all things to all men. More than just one way to do things, hence the hybrid modeler, hence a fuller toolkit not limited just to sketches and ordinary features.
Let's hope that NX-6 holds some extraordinary new features to confound the skeptics and the nay sayers alike. That I could look forward to. From what we've sneaked a peek at thus far it's all good, so I'd just like to say that life is all about change, so to fear change is ultimately to fear life itself.
As for the marketers,... really!
S'cuse me if I'm being too cynical, but anything that can speed up anything by anywhere approaching 100 times (or was it 100% you know the very slight difference between twice actually and whatever it was "up to"); I mean to say I can't think 100 times as fast so what is the point. Take word processing for example; just because computers are 100 times faster than they might have been when Word was first released doesn't change the fact that I can only type about 30 words per minute. The old saying goes that "There are lies, damned lies, and benchmarks!"
Best Regards and keep Smiling
Hudson
RE: Pro/E user attempting switch to UGNX
That's a great thought and one that any marketeer worth his superlatives would be proud of, but the reality is that the term 'Uni-' came from the fact that the company that originally developed 'Uni-graphics' (which BTW WAS the original name of the product including the hyphen) was named 'United Computing Corporation' out of Carson, CA (later acquired by McDonnell Douglas in 1976).
http://w
(where I took my first CAD class in July 1977)
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
I have been using the tool in more or less the same way that we used Pro/E. This is because the parts we design lend themselves best to a fully parametric sketch-based approach. We make hundreds of little tweaks to parts - no major changes in topology. (Aside - we had a CAD war in the early 90s when when the DEC disk business was acquired by Quantum Corp, an outfit that was using HP SolidDesigner, which was 100% freeform modeling. In benchmark after benchmark, Pro/E beat the whee out of the direct-face modeler. The irony is that PTC just acquired SolidDesigner, so they seem to be interested in the technology, perhaps just to keep pace with NXs efforts).
I'm definitely getting used to NX, but what frustrates me is the attitude that common complaints (sketcher not recognizing off-plane curves) is not a problem. Dammit, I am the customer, and I say that it *is* a problem. Anything that forces me into workarounds that take extra hours of sketch time is a problem. Every other mid to high end modeler can do this with ease. I wish Siemens would be more responsive to enhancement requests. We've asked for some sketcher limitations to be improved two years ago! We've been asking for a Cloning enhancement that walks down the product structure and finds *all* the related drawings and WAVE links. Today, we have to sit down with a BOM and painstakingly find every object manually. This can take hours to accomplish what was 2 mouse clicks in our previous tool.
OK, rant over - John and others here are a great resource and I am grateful to all who have responded to my help requests.
Ed
RE: Pro/E user attempting switch to UGNX
In NX 6 we are introducing something called the 'Relations Browser' that shows you the links of related parts in an assembly (beyond what can be seen in the Assembly Navigator) since it can also show you relationships parts are not part of the existing assembly yet which are linked thru some sharing of objects and/or expressions. And it can be generated by selecting a SINGLE button
Attached below is an image of what one of these diagrams would look like. Note that the areas at the bottom and to the right provide additional ways to see information about individual components or certain relationships. The browser allows different ways of viewing the relationships and for large assemblies you can apply filters or limit the content to certain types of relationships and so on.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
Kind of reminiscent of the ANT circa V10 or 11.
P.S. Yes I had seen the site and had known a bit of the History being first aware of United Computing via UNIAPT back in the day when paper punch tape ruled, (it was just after the dinosaurs died out and we started to walk upright for those who don't remember). But then again the idea behind the name United and the word Universal are linked by a common Latin root, meaning "One", so I think the central idea is something you can refer back to if you care to subscribe to something that I think does describe what users and developers alike ought to aspire to. Mind you I'd be the first to unapologetically concede that if those ideals are tinged by self interest then by all means inspiration should not lack motivation should it?
Ed,
I guess you missed the point of a swiss army knife. They always have that little thing for getting the stones out of horses' hooves don't they! Something you and I may never use but which the Swiss Army are evidently fully committed to.
"Now if I have told you once I've told you a Million times; Don't exaggerate!", When you rant others reading with cooler heads pick up immediately that it doesn't really take hours of time to fix off plane sketch curves. I could make a long list of enhancements as easily as you probably could. If we did we'd not only want different things, but to do the same things in different ways. The one thing that we can't have, because there wouldn't be any point, is to create this CAD system the same as another one. Nor can tomorrows' CAD systems hope to stand against the tide of progress if they stay the same as yesterday's.
Please rant away by all means. An honestly held opinion passionately expressed is understood for what it is by this reader at least, appreciated, valued, and responded to hopefully without offending anyone. I do however harbor some concern that I may offend without intending any harm, simply because it is in the nature of the most strongly held opinions that they tend to extremes and are usually wrong because the extreme view being premised on the existence of an opposite extreme fails to take the other into account. Paraphrasing Socrates "I know nothing except that I Know absolutely nothing!"
Insofar as the army knife ties into anything of relevance to CAD then it must be that to quote you....
"...it may not do every single thing as well as products that focus on one methodology (ie; fully parametric)."
Parameters are a good tool indeed. A means to an end, but certainly not and end in themselves. Not a few posters seem to forget that.
My perspective is that a high end CAD system serves its highest purpose when it is used to its fullest on the most difficult of tasks. Among these I would count surface modeling somewhere near the top. In that discipline we often work with and/or without parameters to create the kind of A-Class automotive and industrial design shapes using different tools some parametric but as often not. My wish list of enhancements would certainly draw heavily on surfacing tools as your might on Sketcher enhancements. At the end of the day the beauty of the pocket knife is that you can use it for a range of things whether they were intended by the designer or not. It is that flexibility that for me adds to the justification for making NX the kind of high end CAD system that it evidently is. I find the non-parametric tools, for surfacing, the direct modeling, and feature based modeling are as often a joy to use equally as I find curve creation occasionally lacking.
Cheers
Hudson
RE: Pro/E user attempting switch to UGNX
Thanks for the preview; that looks nice, especially with the thumbnail views.
What I don't understand is why TcEng can't walk the structure for data duplication. All the relationships are stored in there anyway, so it would seem logical to mine the data there. I know you're on the CAD end and not the TcEng end of the business, so this may not be your area of expertise. FWIW, we are working with the TcEng guys to show them how our previous PLM tool could duplicate an entire product structure, including drawings and all links, with a few clicks.
Hudson -
I'm aware that NX (and UG before that) are absolutely best-in-class for industrial design and complex surfacing. In our business, however, we really don't create anything that consumers see - disk drives just end up being stuffed into a box like everything else in a PC. Our models tend to be castings and funky little plastic parts with lots and lots of features. And I won't debate you on the utility of having the sketcher be able to project off-plane curves - it is a serious issue for us and let's leave it at that.
Our designs get reused over and over again and passed around to different engineers, so it is very important to imbed as much design intent as possible into the model. Parametrics and history have proven to be a good way to capture this intent.
I won't comment much on direct modeling because I am not very familiar with it. I believe HP/CoCreate did some very interesting things with it, and who knows, maybe the industry is ready for a new paradigm.
When we were comparing SolidDesigner with Pro/E, we were able to create some common parts that just could not be modified with a direct modeling approach. For example, we would cut a helical groove (cam slot) into a cylinder with a certain path. The path was developed in the flat state and then 'wrapped' onto the cylinder. SolidDesigner could build the feature, but had no way to change it, because it had no knowledge or memory of how it was created. Pro/E would just 'unwrap' the path for editing, and then re-wrap it.
I look forward to learning more in NX6. This old horse is always ready to learn new tricks.
RE: Pro/E user attempting switch to UGNX
For what it's worth, products that carry the 'Victorinox' brand name, including the ubiquitous 'Swiss Army Knife', are designed and manufactured using a popular CAD package from Siemens PLM Software
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
I myself have been an efficient user of ProE (Wildfire 2) and have now switched to NX5 with a change of jobs. Another note is that back when I was at University I did use UG v18 for a bit, so I did have some experience of the UGS way of thinking. My first quote is that the sketcher feature has improved drastically since v18, where the sketch had to be fully constrained before exiting the feature. Very annoying. Secondly, I believe ProE dimensioning was much better in that the design intent was created in the modeling environment and reproduced 'automatically' in the drawing, thus ensuring design intent. In the world where there are designers and draughtsmen, I believe the design intent will be lost with NX. It was also cool that you could drive the model from the drawing in ProE by just double clicking on the dimension and changing its value. I too am fustrated at not being able to dimension a diameter from a revolved feature as described earlier or referencing edges and lines from other features whilst in the sketcher. I do prefer to use a sketch for nearly all features in NX as it gives more flexiblilty to you modeling ability than using direct features like block, cylinder, pad etc. I would like to be able to create an associative spline whilst in the sketcher. Just a another opinion to add to the mix.
RE: Pro/E user attempting switch to UGNX
If you have a look at the image I attached above, and the description of how you get get the same effect by creating mirrored curves, then you can see that it can be done. It may not be done in exactly the same way as you would prefer, but that isn't the same thing at all.
I don't know what you mean when you say that you can't create an associative spline using the sketcher? I think you'll find that you can within the limitations of 2D curve construction. You can create splines with end slope constraints and dimension the knot points if you care to just as any other sketched curve. What is it that you find lacking?
There are more functions for associative 3D splines and curves in the model which aren't sketch based, but to me the whole argument about design intent and designers vs draftsmen collapses when faced with free-form surface geometry. This I say if only because the dimensioning technique as applies to free-form surface elements is largely redundant, your best course of action is to provide data to the CAM processes.
I don't have the Pro-E background to refute the claim that the sketch dimensions preface the drawing, but while NX has some functions that support this kind of thing it seems to me that the nature of drafting is to require some manual application of dimensions. Anything that makes it easier is to be applauded of course, but most purely sketch based models I would not have thought to be overly difficult or time consuming to draft. In addition it is in the nature of the change the CAD brings about that increasingly less drafting may be required. In that way I see the design intent often best reflected by the model in combination with the choice of CAM process.
Best Regards
Hudson
RE: Pro/E user attempting switch to UGNX
Whilst in the sketcher, if you create a studio spline through points and specify G1 tangent constraint at both ends. Assume the first and last points are constructed from the end points of straight line curves. Well, when you change the angle of the straight lines, the spline does not maintain its tangency.
Regards dimensioning. Of course it is very difficult to dimension free form shapes, but I was referring to non free form.
One thing about CAD packages, there is usually a different way to do things and achieve the same result.
RE: Pro/E user attempting switch to UGNX
UGII_DRAFT_EXPRESSIONS_OK=1
To add the dimensions select Insert - feature Parameters. Pick the sketch and then pick the view, the sketch must be in the same plane as the view you selct.
When you have the environment variable set you can select tools - expressions and then click on the dimension - from the sketch- and change the value. Maybe not as elagant as Pro/e but the end result is the same.
John Joyce
Tata Technologies iKS
1675 Larimer St.
Denver, CO
www.myigetit.com
RE: Pro/E user attempting switch to UGNX
I have tried inserting the dimensions from the model whilst in drafting and found it limited. Maybe my inexperience in usuing product, but I found it a nightmare to move the dimensions from 1 view to another. Say a detailed view. Usually this detailed view does not have the orginal dimension origin in view to select during the move.
I know you can use the expressions to drive model from drafting, but as you say not as elegant as ProE.
RE: Pro/E user attempting switch to UGNX
Yes, that is exactly my impression since I have started with NX. Frustrating, and ultimately dissapointing. NX cannot be all things to all people, but I don't think that statement addresses the issue.
RE: Pro/E user attempting switch to UGNX
Slightly off topic I know, so I do apologise, but the one thing that gets me about Diameters (other than inside a Sketch that it is to be reolved) is that Info->Object and selecting a cylindrical face ONLY returns its Radius. Why ?
Specialty Engineered Automation (SEA)
http://www.sea4ug.com
a UGS Foundation Partner
RE: Pro/E user attempting switch to UGNX
For a short description of what PMI is, go to:
ht
Also be aware that PMI has been adopted by and is being promoted by the major standards setting organizations, as noted in the article above. Therefore don't look at this as being something limited to only NX or even Siemens PLM products, although it is true that our company has been one of the leading champions of getting this adopted as a standard in the industry, and in that capacity has worked very closely with the standards setting organizations since the inception of this approach and it's suggestion that it be taken up as an industry supported standard.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
You were right about the studio spline in the sketcher. I haven't had much call for it, so it doesn't actually bother me, though I can see some uses for it. After reading your later post I tried using it and moving the line only to find that the spline once created is a static entity. As far as I'm concerned this is almost totally useless, and does need looking into. I find that the same feature outside the sketcher works in the opposite manner and is for all intents an purposes superior. In summary I don't know why you'd use the version inside the sketcher as it stands when you can use the other one, but at the same time if they're going to have a studio spline inside the sketcher they might as well have one that works or not at all.
Yes as I said the expression based dimensioning isn't up to much, but the attribute based stuff for hole types and threaded holes isn't bad. As I also said I seldom find it too difficult or time consuming to add a few vertical and horizontal dimensions that would take care of most suitable parts. As the complexity increases surely you'd have trouble positioning a larger number of dimensions automatically, and may have to revert to more manual methods. I can only say that I don't miss what I haven't ever had, but I didn't mean to discourage your idea for what may be a good enhancement to NX in the future. Rather I should ask what does Pro-E do with models that don't lend themselves to any kind of automatic dimensioning, ie free-form or molded products with draft applied can be difficult to draft conventionally. My point being that on balance a lot of our work may not benefit from enhancing conventional drafting, perhaps there is something in the PMI package more suited.
NXMold,
What and why would you want to do with off plane sketch curves? It is a piece of software which probably treats a curve slightly off the plane in the same way as one that is sloping away at a 45 degree angle to the plane. Taking the later case as equivalent what outcome would you expect if you tried to constrain it using the sketcher. The problem that exists is there to be solved according to how you apply the tools to solve it. What solution could you reasonably expect the software to provide? What more appropriate response do other systems provide?
The only curves that I ever use in a sketcher are created withing the sketch and line exclusively on that plane. If I take in curves from the outside I can project them first where necessary. What else is there?
I'm not sure which way you were going with the post, whether you were taking somebody's earlier quote to agree of disagree? What I will say is that if you're posting to ask questions or solicit tips don't expect much help if you approach us with a negative attitude. The best way to overcome your frustration is to consider the proposition that other people are happily and successfully making use of this software, somehow there must be some knowledge worth seeking that might make that difference to you experience of it. So why cut yourself off from that experience by focusing on the differences between NX and whatever you have preferred in the past. If this is unfairly directed at you then I apologize, you may take it to be fairly directed at others posting here.
Phillip,
On information about radii.
I think that it has usually been this way, and that it has only become something that I noticed since posters like yourself raised it as an issue.
Interrogating an edge will return a radius and a diameter value. I know that isn't always particularly helpful in all cases, but it may be useful to keep in mind if you weren't aware if it in the past.
Analysis>Geometric properties will return the approximate radius of any surface adjacent to a point that you indicate. Since all faces aren't regular and cylindrical in the case of free-form surfaces for example the value won't always correspond to a diameter. I think that the information on a selected face works on more or less the same principle.
I think what John is referring to above is that this kind of information could and possibly even should be contained within the PMI. The idea there being that design intent and surface topology are treated as two separate things even if they co-exist in the one piece of geometry.
John,
You could comment on the above if I have put the wrong interpretation. I wasn't otherwise sure of where the PMI became relevant to posts made above.
Best Regards
Hudson
RE: Pro/E user attempting switch to UGNX
Now as to why I brought this up in the first place was relative to this idea that somehow it was both critical and strategic that NX somehow allow users to drive feature dimensions from a dimensioned view as contained in a traditional CAD drawing. While much of what we are doing with PMI will assist in the creation of drawings, the real consequence will be that drawing creation will become more automated and thus less critical in terms of being on the critical path in companies work-flows. In fact, many of our customers have indicated to us that their gaols are to move all drawings from the critical path and moving what drawings currently supplies to their work-flows closer to the data models themselves.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
The penny dropped!
Thanks muchly,
Hudson
RE: Pro/E user attempting switch to UGNX
Regarding drawings and not being able to show model dimensions. The inability to simply show feature creation dimesions is what really floored me about NX compared to Pro/E. If I, as a engineer/designer/model creator, am the one creating the parts and assemblies and I have built in a specific intent into the models then I really don't want to have my drafter, who in most cases was not me, to create dimensions for features using references I don't use in my models. If they were to dimension a feature from a surface that was not the same one I used to model the part then there is a possibility the actual machined part could behave differently than the model. At my previous company we probably spent more time up front than most companies in the early stages of product development figuring out how to manufacture something efficiently. We drove that intent into our model/assy creation. We also fully dimensioned, toleranced, annotated, and documented the model in the early stage as those tools were available in Pro/E long ago.
The "wall" between design and manufacturing was eliminated as soon as we started on Pro/E because we determined the overall design/manufacture/deliver process was shortened by doing so. However, the design process was a bit longer because of this collaboration. Initially management frowned upon this when we were not physically creating prototopyes on the shop floor as had been done in the past. When our first physical prototypes worked as they should on the first try, they were soon convinced.
Isn't the whole intent of CAD in general to shorten the ENTIRE design thru delivery cycle? In my opinion it is. If I want to drive intent into my models at the beginning stage because I know it saves me time on the back end then that's what I want to do. I'm not one to "cob" something together at the early stage just to have someone else come behind me and clean it up. That is not an efficient use of the tool.
At this point all I can do is ask questions of people who have used both tools and try to figure out the logic behind the new system. I'm not trying to slam either one, just make comparisions and figure out the best way to accomplish my tasks.
--
Fighter Pilot
Manufacturing Engineer
RE: Pro/E user attempting switch to UGNX
I really hope this observation does not impede the help I get here, you guys are making my NX transition much smoother.
"Interrogating an edge will return a radius and a diameter value. I know that isn't always particularly helpful in all cases, but it may be useful to keep in mind if you weren't aware if it in the past."
I didn't know that, it will help me in some cases. Too bad this is not availible in the measure radius dialog as well.
The PMI arrangement is interesting. We don't use drawings, machinists use a viewer and attach dimensions to the 3d model (parasolid exported from NX) in a way that sounds similar to what you are moving toward. I wonder if there will be (or is already?) a cheap NX viewer (or free, ideally) that would be apropriate for viewing and measuring NX models.
RE: Pro/E user attempting switch to UGNX
Thanks for you well reasoned post. I'll put some perspective into what I mean by getting the most out of the system that may show that we may have different ways of going about things and perhaps that leads to different priorities, or stems from working in different types of industries.
My limited knowledge of Pro-E and other systems besides NX shows that many users are very well organized in their logical processes because it is within the scope of those systems the best way to work. When confronted with the flexibility of NX many find it almost anarchic and prefer to stick to the sketch based modeling that they're familiar with. If you were to tell most operators brought up in the NX way of thinking that they can't use some combination of feature based modeling, chunky solids, direct modeling and in short use it as a hybrid modeler in order to express their desire to model things the way that they think then they would reject the imposition of such limitations. A lot of this comes about because there are a preponderance of older Aerospace and Automotive users for whom the rationale for having UG latterly NX was based in the free form requirements for body, airframe or plastics design, none of which lend themselves readily to conventional drafting. For that type of application most of the time you wouldn't get the downstream benefit in terms of a payoff at the drafting stage regardless of how organized you tend to be. The real payoff is that CAM processes will be heavily relied upon in the manufacturing process and the future if not the present holds possibilities for applying tolerances and GD&T directly to the models so drawings may not even be required. We live in a world that insists that the model and not the drawing is the master.
A big part of the History of CAD and NX in particular was linked to these requirements, because both McDonnell Douglas and Dassault more or less simultaneously adopted 3D modeling technologies to develop new designs that benefited from the application of computing to their design process. Shortly after that they discovered that they were challenged to get this information to their suppliers and found solutions such as CAM combined with NC machining whereupon they made the extraordinarily astute decision get into the business of selling CAD to their own suppliers. Now that is just the opening chapter, perhaps not strictly the way the business arrangements were actually structured, but a fair accounting for what drove the decision making process that saw us progress towards the way we continue to use these technologies even today.
But you know what the good news is that those whose requirements are more aligned with conventional or structural engineering shouldn't think that just because they co-exist with this bigger other reality that means a system like NX shouldn't fully meet their needs. So if you want to work differently by all means do, and in doing so by all means lobby for better features to suit your needs. The bugbear for me is that what seems to get most misunderstood is that flexibility affords you the choice not to use all the tools if you either don't want or need to, whereas inflexibility doesn't have that benefit.
I'm a bit concerned that some of this may sound inescapably elitist so I'd also offer the thought that I've had my fair share of involvement with the straightforward nuts and bolts side of things from time to time and I'd like to offer a though in that vein. My thought is that while you may achieve a time saving benefit from inheriting the sketch dimensions if you take the requirement to think out of the drafters task then the benefit of collaboration with that other individual, a second set of eyes over the design, may be largely lost. I'd hate to see anything that comes about of a modeling necessity translate into an incorrect drafting emphasis by default if large expensive parts or safety issues are involved with the design.
Best Regards
Hudson
RE: Pro/E user attempting switch to UGNX
I agree with you 100% on spending time upfront deciding how datum structures and geometric tolerances be used to embed as much intent into the part as possible. We spent some time training our users (back in '94) on the best modeling practices with Pro/E. The enforcement mechanism was abuse and humiliation of anyone foolish enough to submit a lousy model, which worked fine :)
This ended up having a huge payoff in the ability to pass parts between engineers (typically an issue in history-based systems). We regularly pass designs off, or more often, leverage other peoples' parts into a new design, so it is very important to follow a good practice. For instance, we insist that all features have a descriptive name, because there is nothing more frustrating that seeing a model tree with 200 features named "Extrude".
You will also find that it is really not necessary to use Layers to organize the model, even if it's a complex assembly. NX's Reference Sets are actually a very good way to set visibility of construction geometry of components in an assembly (there John, I said something nice). I suggest you make an effort to use this tool.
We have carried our part design philosophy forward into NX. We use no primitives and our models start with three primary datum planes. So far we have also eschewed direct face modeling. We attempt to always sketch on planes, not feature geometry, which as you know tends to reduce interdependancies between features.
Passing the model off to a draftsman (draftsperson?) does require you to spend some time with them and explain the design intent. Alternately, they can play the model back to understand how it was constructed. I tend to do my own drafting, so I know how the part was structured.
One thing that may help is to construct datum targets right on the model (using sketches with points or small circles in them). This tells the drafter at least where to dimension from. You can add the sketches that define the datum targets to the "MODEL" reference set so that they will appear in the drawing, then view-dependant edit them away in view in which you do not want to see them.
Hope this helps...
Ed
RE: Pro/E user attempting switch to UGNX
If I respond to this it is just to contrast not to criticize. I'll start with just mentioning the background that you mentioned in the first paragraph because the rest is your experience from your perspective and I've certainly had enough to say so I think what you said is all good and I have no problem with it at all. In fact I have no problem with anything you said we just differ in how we use CAD. The point that I would make is how what you reveal in the first paragraph differs from the way we work and the reasons why.
We would differ in how we go about setting up datum structures. This is because we work in absolute most of the time in a CAD sense. In the design sense the datum intent might be to achieve consistent panel gaps or other appearance driven concerns. For that we can set up the part datums as a means to an end and vary them throughout the design process.
Our company would take a very dim view of any enforcement method that involved humiliation and abuse. You can't even tell a dirty joke these days for fear of offending somebody, and getting sued for it. So we have a program to mete out the abuse for us, politely of course. We make good use of checkmate to enforce our modeling standards, we provided some tools to take the drudgery out of organizing some of the data, and we use layers when we need to. We use two standard reference sets one for the Solid Model and one for the Faceted. We do have reference sets in the assemblies but we manage them by means of automatic updates. We eschew any more than that because of the three assembly deep reference set problems that we experienced in the past.
We have been through processes that involved best practices and found that what it usually involved was a generalized list of things not to do, which eventually got chipped away at by exception when no other solution could be found. We have since moved on to shift the emphasis to guidelines that talk about making the data maintainable, so they're all things that you should do, with only a few that you shouldn't. If you also want your designers to be creative and flexible recognize that telling them what not to do doesn't work. The smart ones reject any dumbing down mentality and leave for better paid jobs with your training under their belts. What we say is use the tools that best fit your needs, try to stay parametric, and document your data with naming and collecting it so that others will be able to follow your construction method. Using all the tools holds no fear for us and we have Mentors in the office who get help the newbies when they get stuck. The expectation is to generally raise the standards of expertise and experience to a fairly high level. We also accept that there are final models and studies and that the needs differ between the two, i.e. most initial layouts or studies need not be maintainable.
On straightforward engineering projects I always do my own drafting and I often enjoy it; money for jam
In terms of the terminology that you were struggling with for a concept akin to copying other peoples' designs we tend to use the term "Benchmarking" as code for that. As in we benchmarked several designs and found this one mirrored our requirements, ergo we pinched it
Where this leaves us is with two sets of requirements for different kinds of industries and applications. We also have different backgrounds in terms of how we learned CAD. To me NX is a toolkit which we paid for; I know how I want to use it and I post here because I'd like others to get the same satisfaction from their jobs. I don't think I could ever recommend changing it in ways that suit any narrow application of design when that would curtail the flexibility needed to make a broader range of possibilities happen.
I think John has a few tricks up his sleeve in NX-6 (no pressure...), that will hopefully make us all think differently about how we tackle some of these tasks. What I have seen and he has mentioned thus far makes me realize even hope for some better possibilities to integrate the design data into engineering processes that really by and large bypassed conventional drafting years ago.
Regards
Hudson
RE: Pro/E user attempting switch to UGNX
Our industry backgrounds are somewhat different - as I mentioned earlier, there is virtually no surfacing used in any of our design work.
One of the ways we evolved our current parametric bias goes back to the early nineties when we first started using Pro/E. Before that, Unigraphics was the standard in our industry (minicomputers and disk/tape storage). We used UGII from about 1980 to about 1994. We dabbled in UniSolids a bit (you may remember this was an option in UGII v8. It was great for computing mass properties, but drafting had not quite caught up with the solid modeling capability, so all production work was still done in wireframe.
We had a pretty good idea of how long and what resources it took to develop a product, so when we switched over to Pro/E in 1994 (I believe UG was at V10 around then) we were shocked at how much more productive we had become. Design teams literally went from 6 engineers and 4 designers to 4-5 engineers doing all their own drafting. We have been at these staffing levels ever since. Our management of course still bitches about how long it takes to do things :)
SO we have tended to stick with what worked so successfully for us. Change does come slowly, as evidenced by how long it took for the market to embrace solid modeling. We are probably due for another major shift, as the basic technology as defined by PTC in 1986 is now 22 years old.
I will be very interested in seeing what NX6 has to offer.
Ed
RE: Pro/E user attempting switch to UGNX
Then you may be right when you say...
We are probably due for another major shift,...
...since I think you will find that some of the new capabilities that we will soon be talking about as the NX 6 launch gets underway (April 22nd is the day) will be something that you will want to pay close attention to. Now I warn you that your parametric background (this is NOT a reference to Pro/E, but rather the idea of creating everything with sketches and parametric features) may cause you to react with some skepticism toward some of the claims and even demonstrations that we will be offering, but as you alluded to above, there is a 'shift' coming in how models are going to be modified and updated in the future.
Anyway, keep your eyes, ears and your mind open
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: Pro/E user attempting switch to UGNX
It's been my observation that we've pretty much hit the limits of what can be done in feature-based parametric systems. UIs are improving all the time, but all the waste in the workflow has been squeezed out. CPUs have reduced regen time from minutes to just a few seconds, but you still have to struggle with part history and the challenges therin. IMHO, Pro/E did it to perfection in their 2001 release. Everything since then has been designed to help new users get up to speed more quickly, but there's really been nothing 'new'.
Here's to paradigms!
Ed
RE: Pro/E user attempting switch to UGNX
Hold that thought please.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/