Geometry failing when opening a native SW part

[fcorona]

I work as a mold designer for plastic injection molding tools and I am always at the mercy of the end customer as to what type of CAD data I get and have to build my tools around. We do 90% of our work in Pro/E WF2 but we also have ExpertCAD and Solidworks 2007 for support.

Recently I have recieved some native Solidworks 2006 parts (?? which SP though)and I have the order to build tools for these parts. I've used Solidworks now since 2005 but have never been a heavy user of it for work related tasks so I know my way around it well enough but I am stumped now.

Upon opening this part in either 2006 SP4.1(? on the SP again but it is 4.X) or 2007 SP0.0 the model reads fine and looks good, as the original part designer intended it to, in it's unregenerated state. But the second I hit rebuild I have a lot of drafts and rounds fail on me because of missing faces and edges and the part loses most of it's integrity and functionality. And in this day and age where people dont seem to send real, detailed prints along with their order anymore and just expect us to "make it to the model" I am in a jam because I cant go and edit the failed features when I dont know what should be what.

I cant really get to the original part designer becasue we are subcontracted by another company who is doing the part production. I figured I'd try to find out if there are any known system issues that might be casuing my part to fail before I go to my customer and tell them that their customer just sent us a bad part. I have to assume this model works for them without failure so I need to find out why I cant get it to do the same.

Any help or suggestions?

Thanks,

Frank Corona

 

[CorBlimeyLimey]

Have you tried doing a Save as before rebuilding?

Can you roll-back the FM tree & allow it to rebuild step by step?

Do you still have a problem if doing a Ctrl+Q rebuild?

SW can open native Pro/E parts, can Pro/E open native SW parts?

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[fcorona]

Save-As isnt a viable option in this case because the system exports the model with overlapping geometry. It just so happens that this geometry that is overlapping in the exported file is the same as the geometry that is failing in the native SW file if I rebuild after opening it.

I can rebuild it step by step but the geometry still fails. I am at a loss as what needs to really be fixed though because SW tells me that all the references are gone and I have no good model/print to guide me if I redefine the features to fix the problems myself. I may try to open the model and edit the features before rebuilding to see if I can make sense of what geometry was referenced.

I didnt try CTRL+Q....I always use the rebuild button. I dot know what it does but I'll try it.

And no, Pro/E cant open Native SW parts, at least with the packages we have.

 

[MauricioM]

Can you save this file (parts/assembly) as a IGES/STEP file within Solidworks? Can you do your work around this format?
Do you need all the features (Feature design tree)?
If all you need is the body (dummy) to get the geometry required to create tools, maybe all you need is a different format other than the native file.
Hope this help.
MM

(Mechanical)
Solidworks 06/PDMworks 06
Windows XP Professional 2002
AMD Athlon(tm)64 Processor 3000+
NVIDIA Quadro FX 700

 

[JMirisola]

SolidWorks 2007 has FeatureXpert. Try running that and see if it doesn't help you with your issues.

Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP1.0, Dell M90, Intel 2 Duo Core, 2MB RAM, nVidia 2500M

 

[bvanhiel]

Request a STEP/IGES from your customer. You have no way of knowing the design intent.

FYI, Ctrl-Q forces regeneration from the very beginning of the part. SW usually regens from what it thinks is the last changed feature.

-b

 

[CorBlimeyLimey]

SP1 is now available for SW07. Can you update and retry to open the file?

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[fcorona]

I may try to request a different format but I'm afraid I may not get any better data. From what I've gathered from talks with our customer, the original designer of the part has no real knowledge of what it takes to build the tools to make his part. He just knows what he thinks he wants and wants to make it look pretty. There are so many overlapping rounds (which is a big part of what fails in SW) that even when I do export it to IGES before rebuilding, I end up with that overlapping geometry in my neutral file and I'm sure anyone in here that deals with 3rd party files for tool production knows that that is a bad condition to work with if it is even workable at all.

 

[JMirisola]

Seriously, try running FeatureXpert in SW '07. I haven't had to use it yet but, from what I saw, it's pretty powerful. It just may solve your problems. It will take and reorder your features so that they will work. I'm probably over-simplifying things...

Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP1.0, Dell M90, Intel 2 Duo Core, 2MB RAM, nVidia 2500M

 

[fcorona]

I'll give it a shot.

I'm also in the middle of grabbing SP1.0 with some hope of finding a solution.

Thanks everyone.

 

[Theophilus]

Frank, I've had models from 2006 do this to me in 2007--not sure why--also using SP 1 already (and tried the update wizard to no avail).

However, you mentioned there were lost references. This sounds like the part was designed in the context of an assembly, and that the references weren't properly severed by the client before sending. Your problem may lie here instead of a corrupted file (or something similar). You may want to see if you can check that out.

Ideally, have the client (if you can get access to them) save a part in native format and in parasolid (*.x_t) format. Parasolid will be a dumb solid that won't give you any trouble. (The last thing you need is to start guessing at desgin intent--what if the designer wasn't very intentional? You'll likely guess wrong.)

Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe trumps reason.

 

[fcorona]

Yeah, we may have to get in contact with the original part designer now because I did spend the time going up and down the feature tree and was able to restore the model to a workable state and keep the original design intent and in the process I saw how "rookie" techniques were used to make a model look good but be nearly unusable for manufacturing. The designer used radii that were too big for the adjacent geometry and often engulfed entrie surfaces and previous rounds. Other times an edge would be used that couldnt support a radius along the entire tangent chain so it would feather off into a twisted mess of radii and then to cover this blemished and error filled mess of surfaces the designer would just place a band-aid round over the top if it to try to make it look pretty. Even when done natively in Solidworks, the part refuses to split core & cavity because of the design flow used. Given enough time and a little more information on fit and function of the part I could make it manufacturable and "pretty" but since we are not being paid to do that, my supervisors dont want me to waste my time doing so.

 

[TheTick]

If your customer is working in SW, have them send a parasolid instead of STEP or IGES. Since parasolid is the native modelling kernel for SW, there will be no data lost or mistranslated.

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[TheTick]

BTW, my vendors never get featured SW models from me. Mostly to avoid this exact situation. When I want a quote or a tool built, the vendor gets a file with one model and one configuration, with no features that can change or be lst on regeneration. There is also no reason to clutter up a vendor's hard drive or RAM with feature data he does not need.

I keep an archive of what vendors received which parasolids. File names include a date stamp. When there s a question, it is much easier to trace theorigin of the file in question.

Also, I never build a tool without a drawing to show critical tolerances. I will have vendors quote from just a 3D model, but never build without a drawing.

 

[Theophilus]

I've been asked to make cores/cavities from supplied SW models myself and run into all sorts of nasty hacks along the way. Most of the time it would be faster if I redo the model entirely to set the geometry into some semblance of order (and often it's absolutely necessary since draft is often applied to some faces and not others, with the fillets out of logical order to work properly). Always all sorts of hacks.

If you're one client away from the real client, good luck trying to express this to them. Sounds like the model is junk and the middle client may decide to do the dis-service of assuming you're not competent enough to get the work done. So they'll take the file to someone willing to cheat with the model and ultimately produce an illegitimate tool. (I hope not.)

I use TheTick's methods above to make sure I don't get bad tooling (with, of course, nobody willing to pay for it). If there's a problem with my file, I want to know about it and I'll change it myself. If not, I can be certain nobody will alter my file without obvious signs--since all they'll hold will be a collection of dumb solids.

Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe trumps reason.