Problems Opening a Solidworks Assembly

[TOM S]

When opening a SLDASM (Solidworks assembly model) Mastercam seems to ignore any cuts/trims made at the assembly level.  It seems that it only opens the series of SLDPRTs.  Is there a configuration setting perhaps that can be be set to allow the cuts at the assembly level to be recognized?  

I am running Mastercam 2019.  Not the solidworks version.  We have Solidworks models created by others in the office, and as such I do not have a seat so I can't make a changes to the SLDPRTs.

Any ideas???

[JParis]

Unless something has fairly recently changed, Mastercam doesn't have the ability to read in features created at the assembly level.

[nickbe10]

34 minutes ago, TOM S said:

Any ideas???

Save it (the whole assembly) as a Parasolid Text ( .X_T) file . That will open in MC with all the components on separate levels.

Your SW guys will have to resave it for you.

[Roger]

44 minutes ago, Old_Bear said:

Unless something has fairly recently changed, Mastercam doesn't have the ability to read in features created at the assembly level.

I beg to differ with you.  I make my fixtures by laying the parts on top of the material and converting entities, and doing the cutting in the assemblies..........And the whole assembly opens fine in Mastercam. 

[JParis]

11 minutes ago, Roger said:

I beg to differ with you.  I make my fixtures by laying the parts on top of the material and converting entities, and doing the cutting in the assemblies..........And the whole assembly opens fine in Mastercam. 

Fair enough...I know there was a point in time that was not the case. Apparently it's been addressed

[Matthew Hajicek - Singularity]

I use X_B; it's exactly like X_T but much more compact.

[Pete Rimkus from CNC Software Inc.]

On 5/1/2019 at 2:10 PM, Roger said:

I beg to differ with you.  I make my fixtures by laying the parts on top of the material and converting entities, and doing the cutting in the assemblies..........And the whole assembly opens fine in Mastercam. 

As far as I know, we still do not have the ability to import the result of those cuts when bringing the SLDASM into Mastercam. This has been a known issue for a while and is do to a technical limitation in the libraries SW provides for importing their native files.

Yes - if its exported to Parasolid (.X_T or .X_B) they'll come across to Mastercam, but not from the .SLDASM.

[Roger]

On ‎5‎/‎3‎/‎2019 at 6:32 AM, Pete Rimkus from CNC Software Inc. said:

As far as I know, we still do not have the ability to import the result of those cuts when bringing the SLDASM into Mastercam. This has been a known issue for a while and is do to a technical limitation in the libraries SW provides for importing their native files.

Yes - if its exported to Parasolid (.X_T or .X_B) they'll come across to Mastercam, but not from the .SLDASM.

Maybe I'm not understanding the question.  Please see attached Mastercam file where I built the base piece in Solidworks, built the block 2 in Solidworks, I then did an assembly in Solidworks by laying block 2 on block 1, edited block 1 in the assembly file by doing an extruded cut, using block 2 and converting the edges.  Saved as an Solidworks assembly, and opened in Mastercam. 

Block assembly.mcam

[Roger]

Here is a screen shot from the Solidworks assembly file showing the history tree.

[TOM S]

So here is my update.  I had my SW guys save it out as a Parasolid and it worked fine.  Having not been aware of this issue before, I now see how it has created problems for me in the past.  When I brought in an SLDASM and disassembled it in Mastercam assuming it was the same as I had seen in the SLDASM.  This explains some errors we have had assembling some parts.  Now I know, so hopefully can avoid these issues in the future.

Attached is a zip file of the assembly in question.  If you open the SLDASM (SDL Bar.SLDASM) in Solidworks (or eDrawings) look at the perimeter cuts, specifically the outside edges of the center oval.  Then open in Mastercam and you will see that those cuts are not there.

Int SDL Bar Assy.zip

[JoshC]

On 5/7/2019 at 9:46 PM, Roger said:

Here is a screen shot from the Solidworks assembly file showing the history tree.

Roger, this will work since all of the features were done on a part level not on an assembly level. If you had cuts made like i have in the file attahced or in the Image below that are made on the assembly they do not come through. Easy work around is to save into another format and then you can open it properly.

test.SLDASM

 

[JoshC]

4 hours ago, TOM S said:

So here is my update.  I had my SW guys save it out as a Parasolid and it worked fine.  Having not been aware of this issue before, I now see how it has created problems for me in the past.  When I brought in an SLDASM and disassembled it in Mastercam assuming it was the same as I had seen in the SLDASM.  This explains some errors we have had assembling some parts.  Now I know, so hopefully can avoid these issues in the future.

Attached is a zip file of the assembly in question.  If you open the SLDASM (SDL Bar.SLDASM) in Solidworks (or eDrawings) look at the perimeter cuts, specifically the outside edges of the center oval.  Then open in Mastercam and you will see that those cuts are not there.

Int SDL Bar Assy.zip

Do a save as in solidworks and save as Parasolid or step, if you open those formats it will bring in everything.

[nickbe10]

4 hours ago, TOM S said:

So here is my update.

Just use Parasolid as a file transfer protocol and forget fighting this stuff. You will end up with a million  " work arounds " for all the various problem children (SW isn't the only CAD system). Parasolid is simple and bullet proof.

[Roger]

48 minutes ago, JoshC said:

Roger, this will work since all of the features were done on a part level not on an assembly level. If you had cuts made like i have in the file attahced or in the Image below that are made on the assembly they do not come through. Easy work around is to save into another format and then you can open it properly.

I now understand how your doing your cuts.  You do it by inserting a assembly feature.  I do it by right clicking on the part I want to modify, and click on edit part.

My way it carries through to Mastercam, while your method doesn't. 

The square boss, and round boss, fillets where added my way.  The extruded round cut on the front done your way.  As you can see in the follow images.  All features show in the Solidworks image, but not in the Mastercam image.

Thanks for taking the time to help me understand what the OP was saying.

[TOM S]

17 hours ago, nickbe10 said:

Just use Parasolid as a file transfer protocol and forget fighting this stuff. You will end up with a million  " work arounds " for all the various problem children (SW isn't the only CAD system). Parasolid is simple and bullet proof.

This is what we have opted to do.  The down side is that we use eDrawings on our shop floor for our assemblers to view these models.  eDrawings won't recognize Parasolid files, so our SW guys will have to save out both file types.  Not the end of the world.

[nickbe10]

1 hour ago, TOM S said:

so our SW guys will have to save out both file types

In situations like this I always promise to cry myself to sleep for a week in honor of their sacrifice.....