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Solidworks to Pro E Wildfire

IDseekay

New member
I have tried importing Solidworks *prt files (parasolid)to Pro E Wildfire.My supplier seems to think it would make no difference if they export Pro E prt files. I am yet to trythis.


1) So far, the only option that is producing anything I cansee is the iges export. The problem is, I can only extrude (cut) into some of the parts. I have tried solidifying some componentsin the assembly with no luck. Any ideas?


2) The iges files produce a series of quilts. Does anybody know how I can use these quilts?


3) I just want to be able to manipuate - extrude (cut) etc - the iges data, going from Solidworks to Pro E Wildfire. Any ideas?


I have just started using this platform, so any reply would be useful if you could explain "how to" aswell
 

marker4x4

New member
Ask your supplier to send you their models in STEP format; STEP is much more "rigid" than IGES.



SolidWorks generated (save_as) ProE files are another options, however it's not bulletproof either.



I hope it helps
 

IDseekay

New member
Hmm, yes tried step - WF fires up, but nothing - just an empty working directory. Doesn't even open it up. When I try to navigate to the directorywhere the step file is, (I can see "all files") the step file does not show up on the pro E browser. I have tried opening it the other way round ie right-clicking and "opening with" WF directly - again won't open. There are no problems with the step data itself - tried severalstep files - same result.


a) What I reallyneed is some advice on how to manipulate the iges files I have. Why some parts I can cut, others I can't?


b) Could this be due to the "facet size" of the import?



c) Can I change the facet count of an iges filein Pro E? Would this help me to manipulate it?










Edited by: IDseekay
 

mgnt8

New member
Accuracy is another important issue. It helps to have the accuracy of the model from which your imported data came from match the accuracy of the model you are importing into. If you open the IGES file in Wordpad, in the header, the 20th or 21st item shows the accuracy of the model that the IGES came from. This will help you bring the imported data in as a solid instead of quilts with gaps. Also some config.pro settings that may help:


ntf3d_in_close_open_boundaries yes


intf3d_in_enable_layer_join yes


intf_in_external_accuracy yes


intf_in_keep_high_deg_bspl_srfs yes
 

dalex

New member
If you are in Wildfire or Wildfire2.0 try opening the Solidworks file directly into ProEngineer.


#File #Open
 

IDseekay

New member
mgnt8 - erm...I tried opening up wordpad. Bit confused really, alot of data.
Not sure what I was looking at in the header to be honest.


Could you possibly run through how to import the data as a solid rather than quilts? I think that might be useful.
 

Pommares

New member
To Dalex


Was very interested in your open file directly from SolidWorks approach; as I have tried the Iges conversion; it works but doesn't let you manipulate the object parametrically. So I "open new file" and go to my SW directory. There it appears as blank except for that one Iges experiment; even if I set the search to "All files".


How do I get it to show the SolidWorks part files in the WiFi "open file" dialog box?
 

dalex

New member
Pommares


Wildfire and Wildfire2.0 both have the facility to import parasolids files. To see a list of the file formats ProE can handle. #File # Open and hit the pull down button scroll down to Parasolid, the Parasolid formats are listed there. Alternatively create a new part#Insert # Shared Data #From File and a pull down is available in the dialog box.


The Parasolid design intent cannot be accessed. So you will not be able to manipulate the features.
 

Pommares

New member
Dalex





Thanks for your reply. I truly appreciate the help.


Yes, on your advice,I did get it to list parts as parasolids.


But this entails previously saving as such, just like for IGES.


In both cases I can't really continue work on the part, like redimensioning the sketch or the extrusion. So for practical purposes I can't convert and keep on working. Is there any way to save the parametric data and continue development on the parts. I don't mind redoing the assemblies, but I would like to recover the design sequence for the individual parts.
 

airion

New member
STEP files are definitely the way to go, they are far superior to IGES in this case in my experience. Here's why it didn't work for you. ProE does not recognize the file extension .step, it has to be .stp and also does not like spaces in the file name(this may have changed in WF2).

So for example if you get a file called:
"part one.step"
You need to change it to
"part_one.stp"

Now Proe can import in just fine. The best method is to create a new file, then Insert>Shared Data and choose the file. This doesn't give you parametric data but it should be solid so can cut and protrude new features on it.
 

Pommares

New member
So if that is the best alternative, you are implying that there is no way to continue work in full parametric fashion on a project started in the previous environment?


By the way, what you just described can be achieved equally well through an IGES. Maybe with less consistent results,; I don't know for not having tested extensively.
 

airion

New member
There is not any way that I know of to do a feature based translation from another program into Proe using a standard package or anything else from PTC. I think their are some 3rd party software companies who claim they can do this. I have not used any of them and do not know how much costs are involved.

Back to IGES vs. STEP. In my experience, most iges files can be imported in and look fine when you are in shaded mode. But switch to wireframe and often times you will see yellow and magenta colored lines indicating incomplete quilts and a model that is not solid. Sometimes this is good enough, but if want to add or remove material, check the mass properties, or do any finite element simulation you need a solid model. For me STEP files have translated much better.

So in response to your comments, yes, a good iges translation and a good step translation are basically equal. I just find good iges translations to less common. But this can vary by the program that exports it.
 

Pommares

New member
Thank you Airion. That was quite helpful, although a bit discouarging. In effect, I had only viewed the IGES files in shaded mode. As the features didn't get imported I didn't go ahead and actually work with the objects. So I guess it'll be step/stp.


Anybody out there know who these third party converters are that import features along with the object? Comments on effectiveness and cost would be welcome.
 

dalex

New member
Pommares,


No you cannot access the design intent of the Solidworks part. You can however add to it with Pro/Engineer features and continue developing the geometry.
 

erikmjuntunen

New member
Sometimes depending on the cad system, once you export the file to step format, you must modify the file format from .step to .stp before importing it into Pro/E. That is what I have experienced when using Pro/E 2001. Once you change the step file to a .stp file, it should appear on your list.
 

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