SolidWorks and ProEng 2

[cirus30]

Hello,

I am new to 3D modeling (with some knowledge of SolidWorks now) and was wondering if ProEng is better or if they are both the same?
I know that this is a SolidWorks forum but a fair point of view will be appreciated )


Thanks

 

[bvanhiel]

Pro/E has a copygeom feature that allows you to pull only the selected surfaces from one model to another without a huge amount of overhead. It makes working with large assembiles of related parts (like a swoopy plastic housing) much faster for both the processor and the user.

This feature alone drives me to use ProE on large projects with lots of surfaces.

-b

 

[takedownca]

CopyGeometry is a great feature with a lot of flexibility. However, you can get some of the same functionality in SW by using the Insert Part command.

 

[bvanhiel]

No you can't. Insert part pulls the whole geometry of the part into session which slows down the computer. Having 5 or six child parts of a master having used insert part will create a noticably slower machine. Oh, and insert part won't pull in sketches, so you have to create surfaces to pull relevant reference goemetry that might have been better represented with a sketch, further slowing your regens.

Copygeom only pulls in the surfaces that you need. It doesn't pull the parent part into session. In an assembly where dozens of parts may reference the master it makes a big difference.

Believe me, I have no love for Pro/E, but this is the one area where SWX just doesn't measure up yet. Unfortunately, with their (and seemingly everyone elses) trend of piling on features rather than speeding up the software, I doubt they ever will. Unfortunately it seems that Moore's law is having trouble keeping up with SWX.

-b

 

[takedownca]

Relax, BV. Like I said, Insert Part replicates some of the functionality of Copy Geometry. I didn't say it was a feature for feature replacement. Yes, it's slower, can't import only selected faces, bla bla bla, and so on. However, if you're going to do top-down design in SolidWorks, it's one of the most stable methods. If you can't kill a bear with a .45, sometimes a 9mm will do just fine.

 

[bvanhiel]

Sorry if I came off a bit harsh, but them's the facts as I see 'em.

Of course Insert Part replicate some of the functionality, but there's lots of ways to replicate some of the functionality. You could export iges, you could make assembly references, you could painstakingly copy all of the dimesions from your surface model... but none of them are anywhere near equivilent to copygeom for complex multipart assemblies. I'm talkin' 30 min regens on stuff that takes Pro/E (on the same machine) less than 3 min.

Don't imagine killing a bear with a .45. Imagine killing an elephant with a .22 pistol. Possible, but it's going to take you many times longer than with the appropriate tool. I gots me 2 hammers: SWX and ProE. For jobs that call for big assemblies of surface intesive parts, I pick ProE. For just about everything else I'll choose SWX.

 

[AnnaWood]

Just an FYI, in SW2008 you can import sketches when you do an insert parts. Plus a few other things. Much improved over previous releases.

InsertPart01

InsertPart01

See attached

Anna Wood
SW2008 SP4.0, Windows Vista SP1
IBM ThinkPad T61p, T7800, FX570M, 4 gigs of RAM

http://designsmarter.typepad.com/solidmuse

http://www.phxswug.com

 

[bvanhiel]

Thanks Anna. I'm still on '07 and WF2. We will move up to '08 and WF3 when our customers demand it. I understand there are a lot of fixes in both. The ability to import sketches will help streamline workflow, but won't help the regen issue much.

-b

 

[mjcole]

Anna,

Good mention of Insert Part which is the tool for any Pro/E users to use to allow functionality similar to Copy-Geom. It allows importing Absorbed unabsorbed sketches Surfaces Solid Planes and all else. you can then insert Delete Body or Delete surface commands to show only the geometry you need to reference. You can also create Configurations with each of the entities or features needed by the referencing part to replicate what the copy geom would do.

Not to mention anything more than the following. SolidWorks Sketch tool is Far Far superior to Pro/E's one. Pro/E forces ellipses to Horizontal and Vertical Major/Minor axes. Sketched Splines can provide Curvature continuous transitions and You can add dimensions to splines in 3D sketches which is a lot better than having to drag points to the location you want. Mentioning the 80s Pro/E is still stuck there.

If you want file names to max out at 31 characters and not allow spaces in names and like being alerted about minor problems in the model and constantly fixing mistakes, SolidWorks lets you do things right the first time. SolidWorks lets you design as you go whereas in Pro/E you have to think things completely through before starting if you'd like to finish ontime.

I started on Pro/E and used to do QA work for the company so it doesn't faze me much but everyone should at least try the different programs out to see what suits there needs. However SolidWorks provides more Bang/Buck functionality wise and is constantly adding new Functionality where Pro/E is trying to fix or create new barely usable functionality.

SolidWorks can import Pro/E parts and recognize features where as getting Pro/E Wildfire 4 to recognize SolidWorks parts gives some you imported this wrong message. Wildfire 3 contains no real improvements over WF2 except maybe fixing a few bugs and better than crappy sketch performance.

SolidWorks Patterns are also more flexible than WF patterns because you can suppress them without suppressing their originating feature.

Michael

 

[bvanhiel]

Michael,

You can spend all day picking apart individual software features. I could create long lists for both ProE and SWX. Most of them are just preferences that don't keep me from getting my job done.

I spend some of my time working with large surface intensive models. I am quite versant in both Pro/E and SWX as I don't always get to choose due to customer needs. I find SWX superior for "fast and sloppy" work. It has all sorts of great surfacing tools that create good looking, but poor performing surfaces (poor offsettability and extendability). For anything more than 6 parts referencing the same master model, it's Pro/E hands down. The faster regen times make up for any ease of use advantage that SWX might have.

-b