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ProENGINEER vs SolidWorks

Page history last edited by David Maltz 12 years, 9 months ago

Original Question to the design alumni list:


Hi all,

Here at Novartis (ex-Nektar/ex-Inhale) we have been using Pro/ENGINEER for device design for a long long time.  Now that we're part of a (much) bigger parent, we're being asked to consider using SolidWorks for new projects going forward.  The motivation, as I understand it, is mostly standardizing to better facilitate global project teams.  If only 1 type of software is needed for all mechanical design, it's easier to ensure that designers in the US, Switzerland, UK and beyond can collaborate.

My sense is that momentum is on SolidWorks side, but I'm an old died-in-the-wool Pro/E guy, and I don't want to give up anything crucial for convenience.  We're mostly designing injection molded plastic mechanism parts, with a fair need for good integration with both FEA and CFD analysis packages.  Our assemblies are not very big - 25-50 parts max.

My questions to those that care out there are:

  • If you've switched (or learned both), any regrets?
  • Anyone switched from Pro/E to SW? or switched back to Pro/E
  • With the most recent versions, are there any significant drawbacks to SW vs. Pro/E?
  • Anyone worked with both Intralink & PDMWorks Enterprise?



Responses in order received - names are hyperlinked to comments:


Adam French

Dave Franchino

Patrick Myall

Grant Cutler

Heather Andrus

Sascha Retailleu

Julie Dahlgard

Robert Miros

Christine McElhany

Beth Cooperrider

Art Sandoval & Andrew Zee (az)

 Adam French

I think youre right that there's a lot of momentum on the sw side. I've worked in an office that had both, and while I never heard people complain that their project was using solidworks, I heard people wailing about wishing their pro-e project was in solidworks. FEA is well supported with sw.I'd be surprised to hear if you had regrets about switching.


(in response to question about crashing & trail.txt)


SW keeps a journal file - I haven't had difficulties with it in that regard. A few years back it made a difference what processor you were running (pentium good, AMD bad), not sure if that's still the case, but not every PC is the same, that's for sure. There are some hardware geeks around here - if you wanted more specifics I could dig some up. Because I'm running parallels on a Mac I get more crashes, but I think that has to do with parallels more than anything.


Dave Franchino

We are a product design consultant and try our best to be tool-agnostic. We run both SW and Pro/E. Our client base continues to migrate, in general, from Pro/E to SW. 7 years ago we ran 12 seats of Pro and 1 of SW. Today we run 14 seats of SW and 3 or Pro. We are a complete "pull"... essentially we run whatever our client runs so I think this reflects a more profound shift.  


In all honesty it has been a long time since I've seen a "new" user of Pro/E although I'm sure they're out there. All our Pro/E users are legacy users. New clients are almost always running SW.


I am generalizing here but I believe you will still find Pro/E to have more sophisticated surfacing tools and finds a sweet spot between products requiring Alias and those which can be "styled" with parametric solid modeling tools. Solidworks surfacing tools have improved greatly but still seem to be lacking somewhat from pro's. I believe Pro still gets the nod in managing very large assemblies. Some of our larger clients managing big complex assemblies (Harley-Davidson, John Deere) still run Pro and show no signs of being dissatisfied.


The general perspective is that SW is much easier to learn and use for a virgin user.


In spite of the better surfacing tool in Pro. All of our industrial designers run Alias or Solidworks. We tried a number of times to get some designers into Pro but it never really worked. If the client has no preference, of our 14 engineers, 10 would prefer to run SW. 2 would prefer to run Pro and 2 are neutral.


My perception remains that Solidworks is an easier to learn package for those people coming from a Windows mindset. Pro/E's interface retains aspects of its Unix heritage. In Solidworks there is virtually nothing to learn from a file management perspective and it makes extensive use of the Windows "right click" functionality.


We occasionally ran Interlink and really never made it work for us. We run PDMworks for almost all our projects - virtually any project with more than one person gets run in PDMwork. Our designers and engineers rely on this tool for configuration management from almost the onset of architecture definition - not because they're forced to but because it really helps them manage multiple designer projects. I personally think it's amazing that someone designed a configuration management tool that is simple enough to use that people actually use it!


We run Cosmos/Works and have found that integration seamless. For us this works better than the old Pro/Mechanica interface but to be honest we've not used Mechancia in over a year. Same story.  We're running CF Design 9.0 for CFD which also seems to interface seamlessly with Solidworks and Pro.


I believe you would find the learning curve fairly straight forward if you need to switch but the most important thing is maintain an open mind of course.


If you'd like to chat at all in person please give me a call. In reading this I realize I come off as a bit of a SW honk which isn't my intent. I personally run both tools.


(response to followup question about stability)


In general I have found little difference in the reliability between Solidworks and Pro/E. Each has experienced (in my opinion) builds which were buggy. Each has evolved to a fairly stable place. It is true that there is no trail file that I'm aware of in SW but I've not really needed to use it the way I often needed to in Pro/E. It has a fairly robust auto-save/recover feature which can be configured fairly easily (see attached) and works just like MS office's auto-save. I putz with this occasionally depending on how complex the model is I'm working on. In fact, having a database management system which is identical to Windows is one real plus in my mind. Spaces in files are fine, right click works, etc.


I will say that our say that many of my Stanford brethren seem to run SW on macs running some form of virtual windows and my guess is that this greatly degrades the robustness.


A couple more comments. In a given organization, Pro/E allows - in fact kind of requires - tremendous configuration and customization. In fact, although I once considered myself to be a fairly strong user, the priority and hierarchy of the config.pros along with your user configurations remained an enigma. If you have a very stable organization with good IT support and dedicated users this can be an advantage as you can configure Pro/E at an enterprise level. From a user perspective however I found simple things like making plotters work or getting drawing formats set up was a real pain. We ended up with a few power users who really drove the tool well and then a bunch of really good designers and engineers who were under-using the tool due to its density. Of course we are a consultant so we had to climb that learning curve regularly. For many of our clients they only needed to do that once. Pro/E really lent itself to hyper-optimization from an enterprise level.


By contrast, Solidworks is pretty darn easy to configure. System options are easy to find and change - Under "tools - options" just like MS office.


I have also found Pro/E's help files nearly useless but maybe that's my own limitation. Solidwords (once again) uses windows help and is easily accessed and pretty useful.


The more I read this the more I realize I'm coming off as pro Solidworks. I guess that's the case.


Here is my bottom line. If there is truth to the contention that your new organization will benefit through collaboration with other divisions then in my mind, then the advantages of standardization on a single design tool will almost always outweigh the incremental benefits of different optimized solutions. If I ran an organization that wasn't a consultant I would insist on everyone using the same tool and roll with the whining. I've fought that issue from both sides for many years and designers will always be tool snobs (I'll stop using Pro/E, Solidworks, Catia, etc. when you pry my cold dead fingers off of it). Final bottom line. Both tools you are considering are very competent, powerful packages that can be effectively used by skilled designers and engineers with an open mind. If there were profound differences the free market economy would find them and make the decision for you (remember ME-30, Vellum, IDEAS, etc??).


Patrick Myall

As you know, I could talk all day about SW/ProE debate.  But I'm beginning to think that the biggest issue is the PDM issue and file mgmt.  Both programs allow you to make good designs (though ProE will get you there quicker if have an office full of highly trained users, SWX gets you there quicker w/ an office full of rookies). But as I've jumped around the consulting world, the biggest inefficencies seem to come from file mgmt/storage/systems. 


Grant Cutler

I used Pro-E with Intralink at Ferrari, and then Solidworks with PDM and Catia V5 at Tesla, and I could not believe how mickey-mouse Solidworks is! It is like Fisher-Price CAD or something.

I would think that CAD people in Europe would prefer Pro-E, it seemed ubiquitous in Europe when I lived and worked there, I never even heard anyone even talk about Solidworks.

I think the advantage with Solidworks is the myth that it is easier to use. But in reality, I think Pro-E and Catia are just as easy. And Pro-E and Catia don't suddenly quit as often as Solidworks, and can handle much bigger file sizes more reliably and rapidly. Even an assembly with 25 parts, as you mention, could easily stall any CAD program to the point of uselessness, if the overall file size requires enough memory. But all else being equal, Pro-E and Catia will deftly handle the big file while Solidworks freezes up.


The drafting part of Pro-E is more effective too- offering more possibilities than Solidworks or Catia, that are much less parametric and much more manual, while at the same time being stiffer- they don't let you do as much as Pro-E does.


I think the key to good CAD operations in a professional environment is good administration. And my experiences with the different programs have been colored by the administrators I worked with. At Ferrari we had two truly excellent PTC administrators for 20 designers, while at Tesla we had two marginally competent admins for 100 or so Catia and Solidworks users.


If your company is already set up and running with Pro-E I don't know why on earth you would change. What does your company hope to gain with an amateurish tool like Solidworks?


(in response to followup)


Just to be clear: At Tesla, Solidworks would stall and crash on much smaller assemblies than a whole car.  Even our motor model, which would open in 5-10 seconds in Pro-E or Catia, was a 5-10 minute wait

in Solidworks.  Our best Solidworks guy had one of those little nintendo gameboy things to play video games on while he waited for Solidworks.


Heather Andrus

We run both of these as many of our clients are on SW and need native CAD. We've found that SW is fine for straightforward surfacing (in fact those pesky rounds are way better). With more complex surfacing we end up spending more time on the project. We have been doing this for about two years now and are charging clients an extra 10% for SW because of the surfacing inefficiencies. Some things are just harder to do. Given that, it is a good package and way cheaper. We haven't done any FMEA on SW, just on Pro. 


Sascha Retailleu

Regarding your question, I've used both Pro and SW extensively. I should note that the last version of Pro that I used in depth was Wildfire 2.0, but I used it every day for a year straight for Cisco. I found the most recent editions of SW to be just a powerful as Pro (esp regarding surfacing, which seems to be what everyone brings up with Pro). We used Intralink & PDM works on projects, and I didn't really like either. Both were kludgey. I've designed tons of parts for injection molding in both programs, and they just have a different paradigm for doing it, equally powerful. That all said, I've found SW to be a much more elegant, seamless interface than Pro/E. It's more intuitive, with better logic as to how you perform tasks.


Julie Dahlgard

I learned Pro/E and did that for 2 1/2 years, switched to SW for 1 1/2 years, and than did both in parallel for 1 1/2 years.


I hate Pro/E, love Solidworks. Solidworks is a lot more stable and straightforward. There's people local in tech support that answer your questions quickly. There are less steps necessary to accomplish your goal. Period. I was extremely proficient in both and did complex modeling such as complex surfacing and sheet metal. The last Pro/E I used was Wildfire 2 I think. I have a student version of Solidworks for my school and small projects - by choice. I love using it.


Robert Miros

1. SWX Very quick to learn for newbies, easy for ProE dinosaurs to switch over ;-)

2. Cosmos is good for individual parts, a little weak for assemblies (but other applications integrate well with SW. Blue Ridge Numerics has a good standalone CFD+FEA package, and Ansys is the big daddy in the market.)

3. New versions of SolidWorks seem to have some crash problems and soak up a lot of memory. I expect this will improve with successive generations and possibly adding some more RAM to our boxes.

4. Visualization capabilities - both for using engineers, as well as operations and marketing people who want to see what's going on - are excellent in SolidWorks.


Christine McElhany 

I've switched back and forth between Pro/E and SW a few times in the last six years (depending on what the client needs or what the rest of the team knows how to drive), and I think the differences between them are getting less.


Yes, Solidworks is generally friendlier and a little easy to learn, but Pro/E offers such control. Surfacing capability used to lie strongly with Pro/E, but SW has done a good job of catching up.


To me, the main difference that still exists between the two is regarding collaboration. And not having to do with PDM-type sharing, but regarding sharing of geometry. Pro/E's tools around data sharing (being able to insert shared data such as groups of surfaces and reference features through Insert->Shared Data->Copy Geom) have always been invaluable to me. SolidWorks still can't touch this and continues to struggle with tools to reference geometry from other parts without actually using those other parts. Pro/E's tools make it so much easier for two people to work on the same assembly. I also really love the control Pro/E allows over layers. This is to me a big benefit by giving me a greater sense of control over my work.


Oh, I also think the Pro/E drawing environment is more powerful than that in SolidWorks. It just seems to handle all the designations a little more professionally, especially if you're having to go deep into GD&T.

That said, for the size of assemblies you're talking about (I've designed similar such systems), SW seems to do just fine, and there's a lot less griping in the office about how hard Pro/E is to use. I guess I don't have a problem with the config.pro.


Beth Cooperrider

I have actually switched back and forth between SWorks and Pro/E for the last 8 years. I can't say I love either one; they generally both get the job done, and I need to use what my clients are using. I still prefer Pro/E for complex surfacing (variable section sweeps and boundary surfaces are unique to Pro/E), but have found SolidWorks to do all the basics (basic shapes/surfacing, shelling and drawings) very adequately. SolidWorks is more responsive if you find a bug (and I've found a lot of them over the years). Pro/E is better at handling imported data (tables, points, etc.), but SWorks is starting to make that easier. A lot of Chinese manufacturers are Pro/E based (one of my clients insisted on Pro/E for that reason), but that is only pertinent if they are going to work on your files. Sharing files with edwgs works with either software, though it is native in SolidWorks.


You probably already know that it's much simpler for people who have used Pro/E to switch to SolidWorks because the user interface is more friendly.


I know SolidWorks works seamlessly with Cosmos, but not sure of any other analysis packages. I've never used PDMWorks or Intralink, but in a big company it might be critical to have some sort of check-in, check-out process with SolidWorks because instead of saving files with a version number, it saves over the old file. I do constant backups to make sure I can go back if need be...


That's my two cents, anyway. I think ProE is still a better package for surfacing, but SolidWorks keeps improving their software, and Parametric doesn't seem to be advancing -- so I think you are right that the momentum is with SWorks.


Art Sandoval & Andrew Zee (az)

  • We trust either software for any job SWX is much easier to use and easier to bring newbies up to speed on (az: It's also very easy to pick up for an experienced Pro/E user.) (az: The annoying thing is the spin/pan/zoom control -Shift/Ctrl keys are reversed between the 2 programs!)
  • Pro/E is more powerful on the surfacing side, allowing more control (az: I'm starting to question this after attending Advanced Surfacing class for SWX 2008. Pro/E's Var Sec Sweep is still more powerful and Traj Par function, i.e. the ability to vary a section mathematically along the length of the trajectory, doesn't exist in SWX. However, SWX has arguably a more powerful Boundary Surface tool. The Loft Surface feature in SWX doesn't exist in Pro/E, and it creates a much cleaner surface on a 3-sided patch!)
  • SWX is much easier to do mechanism design on...the dynamic dragging of assembly components is so good we sometimes export Pro/E to it just to easily visualize movement (az: Amen!)
  • PDMWorks is a breeze to use...haven't tried intralink Pro/E edges out SWX in terms of a master merge capabilities. (az: Yes, there is no equivalent to Skeleton, Copy Geom or Ext Copy Geom in SWX.) SWX has one, but it is more limited and can be annoying.
  • Curves, indispensible in Pro/E, aren't as easily used/supported/respected in the SWX world
  • Libraries of user/supplier parts are more easily found in SWX
  • Pro/E is still what....4X the cost of SWX? (az: Foundation XE + Adv Assy Ext is about 3X of SWX. It's about $18K vs $6K. I think basic mechanism functionality comes with Foundation XE, but not sure.)
  • (az: Lack of mapkeys in SWX. Amazingly, many of my old Pro/E mapkeys still work in Wildfire. Those that didn't I've replaced with new ones. Does SWX support mapkeys?)

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