Moving from SW To ProE. Advice?

Hi all.
For various reasons, we have dumped Soildworks where I work (well, technically we've just stopped paying subscription), and are looking at
changing CAD packages. We are on SW2004, looking at the base package of the latest Wildfire.
From what I've seen it looks pretty good, and I don't see anything that we currently do in SW that can't be done in ProE. Obviously some methods, etc will need to change, but I can deal with that.
I have seen two demos, one canned web-demo, and one where a ProE guy came in and showed us some things. It was refreshing to see things work not-quite-as-expected.*
So, here's what I'd like to know:
-Are there any particular bugs to look out for (please see below for what kind of parts we make here)? Anything killer or that I wouldn't know to ask to see, yet is quite a pain to actual users?** -How stable is it? -Any recommended hardware beyond what PTC recommends/certifies? Real-world memory size, etc. -How is ProE with large assemblies (700-1500 parts/sub-assys)? Stability, speed, etc. -What is creating drawings like? -Anything else I should look for in particular? ie: Questions for reseller, etc.
What we do here: Nearly all of our parts are simple blocks of steel with holes and cuts. There's no surfacing or complex geometry. There are a few simple tubes (bent tubing) and sheet metal parts. Nothing complex. So I'm not going to be pushing the modelling aspects of ProE anywhere near it's limits.
We have a fair number of parts with configurations in SW, and from what I've seen I'd likely make good use of the parent->child parts (similar to SW's base part--sorry, I don't know what ProE actually calls it). These are either one casting (or one blank part) to make several finished parts, which are indential except for one or two features. Any practical limits to this? My application would likely: Base_part->Intermediate_part--->All_the_finished_parts. Changes in Base_part do propagate to All_the_finished_parts, correct?
So basically, I want to know how good this thing actually is. Input from anyone who's used both would be really helpful.
Thanks, John
* Converting an AutoCAD drawing into a ProE model-->Open the model to edit a sketch and change dimensions--->While trying to add reference dimensions, the dim would place in the middle of screen, so we all thought it wasn't actually placing the dimension. Took a while to realize that.
** SW has a pretty bug where if you define a cut as "Offset from surface" the dim appears (in the model and in the drawing) as from the selected surface to the middle of empty space! This is something I wouldn't think to ask a salesman (and they likely wouldn't show me), but which becomes a real PITA when you have guys from the shop coming up to you and asking "WTF is up with this drawing?!"
--
Really, I'm not out to destroy Microsoft. That will just be a completely
unintentional side effect.
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Wow, for simple prismatic parts, bent tubes, sheetmetal, etc. I would stay with solidworks. In ProE you'll enjoy 1.5 to 2x more mouse clicks to accomplish the same thing, not to mention a somewhat less-intuitive user interface. Maintenance is slightly more and is in India (sometimes that local VAR is a good thing). I would ask for a demo license to try out Wildfire for a month before you make the switch.
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Can't contrast to SW, but .....
The ref dim thing (hiding itself in the middle of the sketch) is common and my reactions at first were the same. Makes me wonder how familiar the demonstrator is with the program.
1500 parts isn't a large assembly in Pro/E. Think you'll find speed and stability to be fine.... better define stability: Corrupt files are rare to non-existant (in my experience, breath of fresh air after using Adsk software). Crashing is hardware sensitive as any program, with acceptable hardware I guess you could say it's at least as stable as other CAD programs. Also think you'll find Pro/E doesn't require as much computional horsepower as other programs to get comparable performance (my machine doesn't meet current entry level specs for Inventor and a normal assy for me is in excess of 2000 part instances.)
One thing I'd look into if applicable; working in a multi user environment. Something I don't know anything about, but have seen the question asked and seen few or no answers detailing how to go about it.
I'd definitely go the maint, at least first year, as it'll give you access to a lot of "suggested technique" information that will be extremely helpful while learning the program.
You might want to hook up to mcadcentral.com. It has a lot more traffic than this group.
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Lucky you. I'm not being sarcastic. I mean it. I used Pro-E for around 6 years designing injection molds. Yes the learning curve may be a little steeper but Pro-E, at least with my experience, will do what you want when you want to do it, period. I lost my job last year because the owners tired of the constant challenges of trying to compete with the other side of the world & decided to close the doors. Now I'm doing fixture design with SW. If it wasn't for the fact that fixtures are typically primitive entity components, cubes & rounds, I'd probably quit. I may still do that. SW is a piece of CRAP compared to Pro. The only time Pro failed me was when I did something wrong. Not because of any software glitches. Pro-E is mature & robust to the max. Period. Enjoy man. Mike P.

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A couple of things to watchout for in Pro-E:
1) With tubing, the 'enclosed volume' of the part may cause accuracy problems. You may need the routing module to define tubing, as the part accuracy may not let you define a tube of sufficient thin wall. There is a specific accuracy for tubing. I have not tried sheet metal, but the condition is similar (Very large surface area, small thickness).
2) When opening drawings, the drawing may not be up to date. The first thing you must do is a regen to make sure.
3) The file versioning is Pro-E is good/bad depending on your opinion. The good thing is that Pro-E saves all of the old models. The main problem is that you do not get 'file open' protections like other MS Windows apps when two people try to access the same file. If several people are using the same data, you MUST have Interlink or PDMLink. Also, if you 'backup' a project to a directory for mods, the file version goes back to .1 and must be reconciled manually with the files in the 'public' directory.
4) Pro-E litters the working directory with many files. Use speken purge to clean this up and manage the version numbers of files. http://www.spekan.com /
5) Ordinate dims can fail on drawings, and there seems to be no 're-attachemnet' possible. The only recourse is to re-create.
6) Cross sections in Pro-E must be created on the model first and then shown on the drawing.
7) You cannot measure the area of a cross section in a drawing in Pro-E
8) Hole callout 'notes' are not parametric. You cannot callout hole dims from the drawing like SW.
9) All sketches need a sketched plane and another orthogonal reference for sketching. Secondly, when in sketcher, you will need to define references for horizontal and vertical dims (or a coordinate system) This can be problematic when creating features oblique to the main coordinate planes.
10) Even with Wildfire I, it can take many more mouse clicks to create features in Pro-E vs SW. Starting or exiting a protrusion takes a minimum of 5 mouse clicks to select or close all of the references or dialogs, for example.
11) Pro-E does not integrate well (at all) with MS office. Pro-Table and text editor are not even close to using Excel and Word. There are ways to convert Excel data for use with Pro-Table, but the equations are lost.
You would be best served by using the software for a specified time and creating a project from beginning to end. Some of the options (Pro-Assembly, Pro-Assembly Preformance) may sound similar, but the functionality is vastly different.
This is my $.02 after using Pro-E v19 through WF I and training on WF II. My previous experience is on SW 1995-2001. I do mostly die and mold work with complex surfacing, etc...
Good Luck.
Nick E. wrote:

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