Pro/E to SolidWorks Conversion

[j...@energid.com]

Hi All,

I have a large Pro/E Wildfire 2.0 model that I want to convert to
SolidWorks v2007. When opening the model in SolidWorks, the
SolidWorks converter complains that it can't handle Pro/E assembly
files that use version 25 of the Pro/E assembly format. Does anyone
know of a good path to convert the Pro/E model? I've tried a few
paths, but the mate information is consistently lost.

Thanks,

Jim

[Nev Williams]

Okino do translaters Polytrans is one that springs to mind
http://www.okino.com/conv/imp_granite.htm

--
Neville Williams
Z-Axis Design - NZ
"remove the KNOT to reply"

<j...@energid.com> wrote in message
news:1171562180....@p10g2000cwp.googlegroups.com...

[sco...@gmail.com]

Can you open up the version 25 assembly in a new Pro/E version and
save it to the current Wildfire version of Pro/E? Then it will x-fer
over to SW just fine.

[Ben Loosli]

<sco...@gmail.com> wrote in message
news:1171663269....@j27g2000cwj.googlegroups.com...

Pro/E files since V20 are encrypted so SW can no longer read them.
Pro/E V25 IS Wildfire2.

Try doing a save-as to STEP and importing that into SW.

--
Ben

[Paul Salvador]

Ben,

Yeah, they encrypted the format at around v20 but you and everyone using
SW (2006-2007) can import and export Pro/e R17-Wildfire 2 (files and
assemblies, I don't believe WF3 files are supported and I have not
tested).
Otherwise, most every part I've designed in Pro/e (R12-Wildfire 2) can
be imported as a BREP or Surface rep.
On simple parts, planes/sketches/features can be read in but it's
painful, imho, but useful when you need the sketch/feature to manipulate
but,.. it does not always work well.

And, for the original question,.. the v25 files should import fine and
you never could import assembly mate information.

..

"Ben Loosli" <bloos...@earthlink.net> wrote in message
news:vsDBh.2568$_73....@newsread2.news.pas.earthlink.net

>
> Pro/E files since V20 are encrypted so SW can no longer read them.
> Pro/E V25 IS Wildfire2.
>
> Try doing a save-as to STEP and importing that into SW.

--
Posted via Mailgate.ORG Server - http://www.Mailgate.ORG

[mark Bannister]

Paul Salvador wrote:
> Ben,
>
> Yeah, they encrypted the format at around v20 but you and everyone using
> SW (2006-2007) can import and export Pro/e R17-Wildfire 2 (files and
> assemblies, I don't believe WF3 files are supported and I have not
> tested).

In my experience so far newer Pro/E files do not import, not even when
unencrypted.

Mark B.

[nnmmll]

> newer Pro/E files

'newer' files are Wildfire 3.

> unencrypted.

no idea what that means. exported neutral?

[mark Bannister]

Newer, wildfire 3. Unencrypted- third party decryption is available.
Mark B.

[nnmmll]

> Unencrypted- third party decryption is available.

decryption or translation? Name?

[mark Bannister]

nnmmll wrote:
>> Unencrypted- third party decryption is available.
>
> decryption or translation? Name?

Decryption, Delcam PS-Exchange. Translation as well. Fee based per
usage.

[nnmmll]

> Decryption, Delcam PS-Exchange. Translation as well. Fee based per usage.

they still have some debugging to do? other theories?

[mark Bannister]

nnmmll wrote:
>> Decryption, Delcam PS-Exchange. Translation as well. Fee based per usage.
>
> they still have some debugging to do? other theories?

The only other options I found last year was buying a view/exporter with
a Granite license. Most cases it turned out cheaper to buy a seat of
pro/e.
The latest files we brought in from Wildfire 3 were via step and iges.
The files came in horribly. I don't know what the issue was but we
spent hours repairing them.

Mark B.

[nnmmll]

> The files came in horribly. I don't know what the
> issue was but we spent hours repairing them.

Maybe hook sources up with
http://www.prostep.org/en/services/bp/cadkombi/proengineersolidworks.htm

This is very basic checklist but for most purposes a very basic
checklist is all that's necessary.

Solids are what you want. Verify that's what was exported. No shrinkwraps.
No Geom Chks, at very least none that affect model topology in exported state.
Clear all tick boxes except Solid for export. They might not use absolute
accuracy but should check the export for minimum resolution and verify it
is not larger than 1e-3 to 1e-2 mm. Resolution is written in their export
log and in the neutral file.

HTH

[Cliff]

On Mon, 19 Feb 2007 18:28:20 GMT, "nnmmll" <n...@nn.mmll> wrote:

>> Decryption, Delcam PS-Exchange. Translation as well. Fee based per usage.
>
>they still have some debugging to do?

Anything specific?
--
Cliff

[jimsym]

Paul Salvador is correct: The ProE Converter has "decrypted" ProE
files since SW2005 SP4. SW2006/2007 will convert files from ProE V17-
WF2. The feature-based converter works fairly well on simple,
prismatic parts. For other parts, use the BRep converter. Look up
"converting ProE files" in the Knowledge Base on the customer portal.
There is pretty extensive documentation as to what the converter
supports and what the limitations are.

For example:

"The Pro/ENGINEER translator imports Pro/ENGINEER part or assembly
files as SolidWorks part or assembly documents. The attributes,
features, sketches, and dimensions of the Pro/ENGINEER part are
imported. If all of the features in the file are not supported, the
file may be imported as either a solid body or a surface model. The
Pro/ENGINEER translator supports import of free curves, wireframes,
and surface data.

When importing an assembly, there is the ability to control how to
import individual components. Sub-assemblies are supported as well.

Pro/ENGINEER surface-trim and surface-extend features can be imported
into SolidWorks. These features are read in from the Pro/ENGINEER file
and mapped to SolidWorks.

Currently Versions 17 through 2001 of Pro/ENGINEER and Wildfire
versions 1 and 2 are supported. Supported versions of Pro/E will
continue to update with future releases."

Wildfire 3 will be supported in SW2008.