Solidworks vs UG 7

[PlasticFantastic]

For the last few years I have been banging my head in frustration. The company that I work in we have two sets of engineers. One set uses UG and another team uses Solidworks.

CAD files are given to both teams, but I love it when the Solidworks team is involved because I am a Solidworks user and can hand over native files. When working with the UG team they have to reconstruct the parasolid that I hand over to them (which seems to me like a big waste)

This would not be much of an issue if UG wasnt so slow. From my point of view every feature seems to be nested and calling up top level assemblies seems to be a big problem. Changes in UG take about twice as long as changes in Solidworks. (please proceed to educate me as to what I am not seeing)

Apart from disparaging remarks like calling Solidworks a toy and "Saladworks", I have not heard any solid reasons that UG is better for our purposes (we design a range of products from GPS hand-held to large assembly products 500-1000 parts). If anything- the geometry from SWX we hand over tends to be cleaner! We have robust models that can be modified faster. My team is a human factors engineering team and hand down the ergonomic interface elements down for further detailing.

What did you get for the money that you paid. Perhaps UG needs power users to unlock its power. If anyone can give me good info I would appreciate it very much. Is there a particular threshold beyond which the power of UG is fully utilized?

I feel like I have never been given a straight anser either way and would love to hear a UG engineers point of view. Thank you for your time.

 

[Xwheelguy]

Jason,

I've been creating Class A surfaces natively in UG for close to 10 years & the ONLY time I have to adjust ANY tolerance for Freeform Features is if the curve quality creating the FFF is not what it should be. As a matter of fact, if you go to a UGS-led training class, they will tell you the same thing (so do the folks at Alias). Freeform surfacing in relation to the parent curves is more often than not a garbage in garbage out type of operation. 90% of the time you can take a situation where you've had to raise tolerances & find the problem resides in the curves in some way. Fix the curves & then there is no need to adjust the tolerances.

If you're having to adjust tolerances on features or feature operations as well as Freeform Features, then maybe you need to re-evaluate your default tolerances or techniques (used in UG). I personally would not feel comfortable not knowing what tolerances I was modeling at (tolerances blind to user in Solidworks). Maybe you're modeling at a tolerance that's very forgiving (0.05) in SW compared to a much tighter tolerance in UG....but the fact is, you don't KNOW what you're modeling at, which in my area of usage isn't acceptable. Hence why we're using using UG and CATIA (which by the way makes Solidworks as I'm sure you know, and in v4 the tighest one could model was at 0.01mm but has since been changed to 0.001mm in v5). However, it may be quite acceptable for the parts you are/were creaing in SW.

Like I said in my previous post, it's probably much wiser to invest in a CAD system that fits your needs than a CAD system that is high end only because it's high end & not because you can create parts in it in an efficient manner. If Solidworks or any other midrange software fits your needs, then by all means use it. My personal opinion is that yes, they are very nice programs & they probably come closer than UG, IDEAS & CATIA to being a complete AND affordable modeling solution. However, they sometimes stumble in specific areas when dealing with massive assemblies, large PDM databases, Class A surfacing, machining, non-linear FEA, natural frequency & having the ability of designing a complex part completely through, as Ben said, the concept to final part...it's not just freeform. Sometimes it's because of downstream applications or the complexity of the part being modeled.

I was simply pointing out that tolerances are always used in math-based CAD in some way & that midrange systems don't ALWAYS fit everyone's needs and that is where UG, CATIA & IDEAS fall into place. Unless we all start designing the exact same parts and thinking the exact same way, I don't feel anyone can prove one system is better than another.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[J-C]

To start, our default tolerances are set to .001". Seems a little loose to me but being a SolidWorks user, I've never dealt with it before. I think I once heard that Solidworks tolerance was internal set at around .00000001". Maybe back when UG was getting started and computers were a lot slower, this was a bigger deal to set it low.

Can you elaborate bit more on the curve quality, not sure what you mean by that.

Solidworks would work here as we don't do large assemblies or class a surfacing, but there's a lot of legacy UG stuff and I don't have much say in the matter anyway.



Jason Capriotti
Smith & Nephew, Inc.

 

[Xwheelguy]

Jason,

Regarding tolerances, it's just going to depend on your product & the required or acceptable surface appearance. For example, there is more than likely a larger tolerance (like 0.001" [0.025mm] or higher) used when modeling a cast finish engine part than there is when modeling surfaces to be used on the surfaces used for exterior automotive surfaces like a car body, interior surfaces (dash, seat, etc.) or even visible wheel surfaces. The appearance isn't as critical to the cast engine part, therefore the tolerance may be able to be loosened up a but (made larger). If you're using the 0.00000001", that is even tighter than what is used in Class A surfacing (at least in the automotive application). I would consider 0.00254" (0.0001mm) to be very tight (and difficult) to model in UG. We use 0.0254" (0.001mm) for our surfacing & rarely have any problems (such as having surface edges show up) when we cut our models into wood composite for verification. That is entirely preference, not fact. It might be good for you to read some of the tolerance-related posts on the UG BBS Notes webpage or even post a question relating to the usage of tolerances in UG to get a better idea of what might fit YOUR application. I can't speak for SW though.

I'll do my best to elaborate on the curves, but it's difficult to transfer that into words. Also, I'm not claiming this as "law" for freeform modelers, this is just what I have been instructed & practice, but may conflict with information other folks have learned or practice when using UG. Also, some of this information may be word for word from the UG Industrial Design training manual. The problem here is trying to explain this without visual examples for you too see what I'm talking about. And there is quite a bit of material to explain. Due to time constraints, I may have to respond in several posts at different times.

Basically, if you do not pay close attention to the characteristics of your curves when surfacing (like spline degree & segmentation), then you may have a difficult time predicting the results that you will get with your surfaces or with secondary or tertiary surfaces (such as blends or blend surfaces). Surfaces inherit their degree & patch count directly from the curves that are used to create them. In certain instances, if a spline's degree is too high or the segment count is too high, the resulting surface may appear to have discontinuities. Or if your parent curve(s) have too low of a degree or segment count, the surface may deviate (be further away) from the general shape of the parent curve(s) or be very difficult to control the desired shape/look of the surface. Really it just depends on how strict you need to be with the quality of surfaces.

"Splines have a degree and a segment count. The number of poles is related to both the degree and segment count. A spline will have AT LEAST one more pole than its degree. (A 3 degree spline will have at least 4 poles but could have more poles). If you know the degree of a spline, you can calculate the number of segments" as follows: # of poles - degree = # of segments. Also, the higher the # of segments in a spline, the closer the spline will be to the poles.

Based on the calculation above, a 3 degree spline with 5 poles will have 2 segments. This type of curve is quite easy to work with. But a 3 degree spline with 10 poles will have 8 segments, which will make the curve closer to the poles, but more difficult to manipulate because of the high number of segments. The higher the number of segments, the higher the patch count in your surfaces, which CAN (but not always) cause problems when editing or create discontinuities like ripples or dips in the surface. So, if you're not paying attention to your curves, then any problems you may be having with surfaces might trace back to the curves themselves.

Other modeling techniques can also come into play when it comes to tolerance issues. For example, if you're creating surfaces, make sure they pass completely through any bounding surfaces that you may use to trim to later on. If at all possible, avoid trimming to edges & trim to faces or bodies. Edges have tolerances & you also set a tolerance to a Trim. Using an edge as a trim boundary MAY (not always) lead to tolerances stacking up & increasing more & more as you get further along in your modeling. I know that sometimes it's impossible to avoid using edges as trim boundaries and that's fine, but if you can, then by all means avoid it.

I would recommend playing around with curve quality, specifically spline quality and the resulting surface degree & patch counts. Keep the degree for splines as low as you can (3 deg. min. & 5 deg. max with maybe 7 deg being the absolute stopping point). Keep the segment count for splines as low as you can. This will sort of cause you headaches at first, but once you get a feel for it, you will begin to see the results in the surfaces & eventually get a sort of "feel" for it. Use your analysis tools in UG. Look at the splines, the curvature combs, the segments, the degree/segments of curves vs. resulting surface degree/patches. You should start to see what I'm talking about if I've explained this well enough. I'm not a very good teacher unfortunately.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[J-C]

Thanks for the explanation but the spline degree and segments has me a bit baffled. What exactly is a segment?

In solidworks, splines have no degree, or no option to specify one. You just click the points where you want them. If you want more you right click it and insert one, if you want less you select it and hit delete.

Jason Capriotti
Smith & Nephew, Inc.

 

[Xwheelguy]

Jason,

I'll have to do some research on giving you a straight definition of a spline segment. I don't want to pass along inaccurate information.

I find it quite interesting that SW doesn't place as much importance on the splines or the information about the splines as UG does. Maybe the folks at SW just didn't feel that complex surfacing was something they wanted to get into & wanted to keep things as simple as possible. I would be willing to guess that by default SW models with 3 degree splines just to keep things standardized. It could also have something to do with the level of math that the entire software is based upon...maybe it just can't handle high order curves & surfaces as far as creation is concerned. Would be interesting to know the details.

It DOES get difficult when you begin working with higher degree splines & surfaces in any software....at least in terms of knowing what sort of behavior to expect when using certain types of splines & the nature of the resulting surfaces.

Also, please remember that when I explain details of modeling, I'm speaking in terms of UG only. Other softwares may or may not be similar or they may or may not place as much emphasis on the curves side of things. It all just depends on the tools you have to work with & the intent of the software.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[cowski]

To boil it down, a segment is a spline. UG allows you to specify the degree of the spline along with as many defining points as you like. To pull off this trick it joins multiple splines. The number of poles -1 = degree of spline; so if you want that 3 deg spline but use 5 poles, UG will make 2 3 degree splines and join them (2 segments). If you do an info object on this spline you will see it has 1 c2 knot, this is essentially the point where the 2 splines join (they must be curvature continuous to have a useful single spline).

 

[Xwheelguy]

Thanks cowski. I wasn't sure how to describe the joining of the spline segments in terms of the continuity.

Do you happen to know what characteristics would result in C0 or C1 knots being applied to a spline? At a glance, it appears that it is degree/pole related, as I opened UG & created a 2 degree spline with 4 points & the resulting spline had 2 segments with 1 C1 knot. It's been a while since formal training, but I'm thinking that if you lower the degree while increasing segment count then the spline will lie closer to the poles & be "stiffer" due to the decrease in type of continuity assigned to the knot(s).

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[Azrael]

About spline degrees, a 5 degree multisegment spline will get c2 continuity. Prefered for styling if you don´t use single segment splines.

This is the first time I ever heard someone state that solidworks is better then UG in advanced surfaces. I´m wondering if he really talkes about advanced surfaces as class A.

About tolerance tweaking, the only time I need to tweak it is when get bad data to work with.

I´m working with UG, Catia V5 and alias, I have tried Solidworks, solidegde and inventor and must say that if you with non complex parts the three last mentioned system works just fine but when it gets complicated they aren´t in the same league

 

[Azrael]

Correction:

"About spline degrees, a 5 degree multisegment spline will get c2 continuity. Prefered for styling if you don´t use single segment splines."

It is C3 continuity

 

[J-C]

We don't do Class A surfacing. We also don't have a license of the Studio surfacing so we are just using Freeform and thus I can really comment on what functionality may lie there.

UG does indeed have more tools for creating curves and surfaces than Solidworks. Solidworks is just easier for most stuff I've run across here, at least what I've found when I go home and try modeling it in Solidworks. Something that I and even an experienced co-worker struggled to get to work in UG was a breeze in Solidworks. Also I never done much freeform surfacing even in Solidworks so there's a learning curve there too.

I'm not here to UG bash, fact is I work with UG so I'm trying to make the most of it.

Jason Capriotti
Smith & Nephew, Inc.

 

[cowski]

The knot type is degree/pole related. If you make multi-segment 1 degree splines (a line, 2 defining poles, 1 at each end) the best you can get is c0 knots (position). Multi-segment 2 degree splines (3 poles) can get c1 knots (tangency). Multi-segment 3 degree splines (4 poles) can get c2 knots (curvature continuous). The spline definition is based in part on polynomial equations, the knot type is a result of taking derivatives of these equations. The derivative of a 1st order equation, a line, is a constant (point, or c0 knot). The derivative of a second order equation (or higher) gives the tangent, etc. This is why you can't get c3 knots in a degree 3 spline, that derivative doesn't exist.

The knot type can also be a result of using 'join curve' indiscriminately. For example, if you draw a quick rectangle and use join curves on the 4 lines you will end up with a degree 3 spline with c0 knots. Be careful with 'join curve', it gives you what you ask for - not necessarily what you want.

if you lower the degree while increasing segment count then the spline will lie closer to the poles & be "stiffer"

It is true if you lower the degree, the spline will lie closer to the poles, however, (to be consistent with the UG docs) I would call this spline "looser" (or maybe "pliable"). UG documentation defines a stiff spline as one that doesn't lie close to the poles (ie a large change in pole location results in a small change in the spline). I wouldn't recommend using anything lower than a degree 3 spline, and if you do high end class A stuff (I don't) you may want to use degree 5 splines as Azrael has suggested.

Regular splines in UG only report c0, c1, and c2 knots but a degree 4 (or higher) spline could technically have c3 knots. I wonder if knots higher than c2 are simply not reported or if you can only get them using studio splines?

 

[Xwheelguy]

I know what you mean in regards to Join Curve resulting in undesireable splines. I have found that the same problems can arise when using Project Curve & Intersection Curve.

I really like the Shape Studio Curve on Surface, but it lacks (at least in NX2) the ability of assigning continuity across multiple surfaces.



Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[Dave K]

Since the discussion has turned towards splines...

Using UG NX, if you put in a spline by poles, and select "single segment", the curve degree option grays out. Is the degree of the spline then driven by the number of poles? ie Poles-1=Degree

I'm curious because in the "good spines" tips, it says:
* Use single segment splines whenever possible.
* Use degree 3 splines when possible

-Dave
Everything should be designed as simple as possible, but not simpler.

 

[ewh]

Gunman,
I believe this is limited by the mathematics used, not by the software. A similar question was asked some time ago in this forum, and nkwheelguy (I think it was Tim) posted a very good explanation.

 

[Dave K]

Reading a little farther answered my own question:

"Notice that the curve degree and closed curve options are no longer selectable. The curve degree will be derived from the number of points used to create the spline"



-Dave
Everything should be designed as simple as possible, but not simpler.

 

[karthikj]

What About UG open ?
No other cad package has this much functionality if we go for automation work.With 4 years of experience in UG i definitely believe that UG is the best for customisation work and all other packages are years behind UG in this field.
For repititive kind of work and customised model creation no other CAD package can beat UG. With Knowledge fusion adding power to customisation work definitely UG is my Choice .

Thanks,
KarthikJ
QuEST

 

[Xwheelguy]

Off the current topic a little, but I made a mistake in an earlier post. I stated that a 3 degree spline with 10 poles would have 8 segments. The spline would actually have 7 segments, not 8. Sorry for the mis-information. ;o)

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com