How to import ProE files in Solidworks

[Tony888]

I imported a file (attached) into Solidworks in many difference ways. However, I only have it as block ("imported") which I can not sketch edits or modify the part. Can anyone open it in Solidworks and share with me how to get its sketch and enable to modify it? Many thanks

[DareBee]

A dumb solid is what you get from any import.
You can sketch, extrude, cut, etc any dumb solid - no problem.
You can also run the SW FeatureWorks module on it, to try and turn it back into a feature based item.

[Mike 1948]

Originally Posted by Tony888 I imported a file (attached) into Solidworks in many difference ways. However, I only have it as block ("imported") which I can not sketch edits or modify the part. Can anyone open it in Solidworks and share with me how to get its sketch and enable to modify it? Many thanks

Here is a SWX 2009 file I ran through the Pro E translator. It came out fairly well requiring only minor cleanup. You will have to fully constrain the sketches though.
I'm real curious how this part is going to be manufactured.

Mike

[JimV]

When you import the Pro-E file. Make sure you check the Features Icon.


To import a Pro/ENGINEER part file into SolidWorks:

Click Open (Standard toolbar) or File, Open.

In the dialog box, set Files of type to ProE Part (*.prt;*.prt.*;*.xpr).

Browse to a file, and click Open.

In the Pro/ENGINEER To SolidWorks Converter dialog box, set these options:

Import geometry directly. Imports a model without features, either as a solid or surfaces.

BREP. Imports the model as a solid using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models.

Knitting. Attempts to knit surfaces during import. Select Try forming solid model(s) to form solids (rather than surface bodies).

Do not knit.

Analyze the model completely. Determines the number of features that SolidWorks can recognize and import.

Import material properties

Import sketch/curve entities

Import geometry from hidden sections

Click OK.

If you select Import geometry directly, SolidWorks imports the model. If you select Analyze the model completely, SolidWorks parses the imported file and redisplays the Pro/Engineer to SolidWorks Converter dialog box with a summary of the features and surfaces recognized and the following options:

Features. Imports the model and attempts to recognize features. Attempt to correct invalid features attempts to correct problems such as reversed extrusions.

Body. Attempts to import the model as a solid using Knitting. Attempt to correct invalid feature has no effect.

Generate translation report. If you select Features, generates a report that includes the features plus the recognition and import status.

Click Features or Body to begin importing the part.

In the Translation Report:

Print

Copy

Close the dialog box to finish importing the part.

[Tony888]

Thank you DareBee; Mike 1948 and JimV so much for your replied. That part is an elbow connector for a gas regulator. The company I work for builds the cookers. We purchased those parts from distributors and I have to draw it up to attach into the cooker drawing. We recently owned Solidworks 09 and need to convert all existed files from our ProE. Your instructions are really helpful and make my work more easy.

I followed the instruction (step by step) by JimV. However I keep having an error at cut-revolve3 and therefore the shape didn't turn out right. I want it to be like the file that Mike 1948 attached. How do I fix it guys? Mike 1948, is your procedure difference with JimV's ?

[JimV]

Tony

See Attached file of the sketch to fix the problem your having.
JimV

[Mike 1948]

Originally Posted by Tony888 Thank you DareBee; Mike 1948 and JimV so much for your replied. That part is an elbow connector for a gas regulator. The company I work for builds the cookers. We purchased those parts from distributors and I have to draw it up to attach into the cooker drawing. We recently owned Solidworks 09 and need to convert all existed files from our ProE. Your instructions are really helpful and make my work more easy. I followed the instruction (step by step) by JimV. However I keep having an error at cut-revolve3 and therefore the shape didn't turn out right. I want it to be like the file that Mike 1948 attached. How do I fix it guys? Mike 1948, is your procedure difference with JimV's ?

My procedure was the same as Jim's. The cut-revolve failure was due to a "single" point being on the revolve centerline. Adding a line like Jims corrects the issue. That was part of the minor cleanup I mentioned.
Remember go back and modify all the sketches to make them "fully defined". If you don't, it will come back to haunt you in the future.

Mike

[Tony888]

Thank you Mike 1948 and JimV very much.

[diycnc]

I am curious as to why you went from pro/e to solidworks? both are very capable cad packages. i actually think you can do more in pro/e, its just slightly harder to use.

[Tony888]

diycnc, the version we are using for ProE is very old and the guy who knows how to use ProE retired from his position. Instead of upgrade the ProE, we rather purchase the latest Solidworks which I am more familiar with. Also, if the company decides to employ a new draftsperson, it is easier to find a solidworks person.