Hello,
I am trying to import a step assembly file in 2013.
Under the options settings I no longer have or see the ability to,
(Import Multiple Solids Parts as Assembly) This was an option to check.
This seems to be a big issue as we always import the assemblies, then ground them.
And this gives us the option of moving or deleting certain components, as well as opening individual
components in their own part environment.
Please advise?
Thank you
Mark E.
Solved! Go to Solution.
Solved by ToniQin. Go to Solution.
Attach the *.stp file here.
It should recognize the file as an assembly or you can always push the parts and assembly out after opening.
I believe there may be a bug in the software.
It is not recognizing that's its an assembly file.
I exported an assembly file as a step, and then reopened it
and it opened fine with all the components in the model tree as separate parts.
I believe it worked because it was originally saved in Inventor.
My problem now is, which I never had before is that it is not recognizing
the file as an assembly and it is bringing in all the components a base features.
Thes are propietary files which I cannot share, but I know they are created in
the unigraphics modeling package as well as some proe.
Thanks,
Mark E.
I have tried every available option and combination of options
as you show in the import options screenshot. After a little more digging through trial and error
we have conclude,(we believe) that the stp translator has a bug or is corrupted
in some fashion. We then tried to import a few parasolid assemblies, and they opened fine.
That is why we believe the translator software is not working right.
The other wrench in the works is, that it is not working on at least 4 workstations.
We are wondering at this point what to do. Software reload?
Thank you,
Mark E.
I've got the same problem, and it only happened under 2013.
Attached is a sample STEP file that exhibits this behavior.
Rusty
Works fine here with the default settings. You may want to check with who supplied the file how they exported it.
Blair & anyone else,
You say it works fine, and I disagree with you.
I can open any assembly (STP.) and get the same result as you.
The problem is, the file you show now is a single part file.
Note the top of your model tree, that is not an assembly icon, it is a part/surface icon
It should be an assembly icon. Try to right click on any one of those base features and open it.
It should open in a new window. You won't even have the option of opening it. When you expand
the model tree (solid bodies) and try to open up one of the base models, it takes you into the Fusion software.
In all previous versions, We had a checkbox in the Step import option that stated,
(Import Multiple Solid Parts as Assembly) It is no longer there in 20013.
If it is not needed there must be another solution to this, or I believe Autodesk dropped the ball here.
Frustrated and still hoping for a solution,
Mark E.
I have added an attachment from old version of inventor, which clearly shows
the checkbox / option which has been omitted in the 2013 version.
Thank You,
Mark E.
Are you sure that the step is an assembly and not a multi-body?
I just created a step froma an iam and it re-imported as an assembly.
Yes, they are assembly files, have been for 8+ years.
If you create it in Inventor and export it, then reopen it
it will work because it was created in inventor.
Its when we recieve files from vendors and customers
who use other softwares when this becomes an issue. (unigraphics, catia, solidworks, etc.)
Read post from beginning thread and you'll understand what were dealing with.
Thanks,
Mark E.
@rdyson wrote:Are you sure that the step is an assembly and not a multi-body?
I just created a step froma an iam and it re-imported as an assembly.
STEP files are not assemblies or anything else. They are solid bodies. There may be multiple solid bodies contained within that single file.
In previous versions of Inventor - at least 2010 and 2011, anyway - when you imported a STEP file containing multiple solid bodies, you had the option of bringing it in as an .IPT with multiple solids, or of bringing each solid in as a separate .IPT within a larger assembly.
Some vestiges of that remain - when you set your import options there's an option to have the individual parts stored in one place and the top-level assembly file stored elsewhere ... but since Inventor won't import the multiple-solid STEP file as an IAM, that doesn't really do anything.
Rusty
If you created it in Inventor, export it, then reopen it, it works.
Thats because it was created in Inventor. Its files created in (Unigraphics, Solidworks, Catia, etc.)
that are the problem now.
Pleas read thread from beginning and you'll understand the issue.
Thank You,
Mark E.
Lt. Rusty,
Please go back to message 9 on the thread and open my attachment.
It cleary shows the checkbox in question which
has been left out in 2013. (Import options)
Thats the magic button we need put back.
That will fix everything that we are discussing here.
Thanks
Mark
@markerdani7076 wrote:Lt. Rusty,
Please go back to message 9 on the thread and open my attachment.
It cleary shows the checkbox in question which
has been left out in 2013. (Import options)
Thats the magic button we need put back.
That will fix everything that we are discussing here.
Thanks
Mark
In case you hadn't picked up on this already, I've been agreeing with you.
Rusty
@markerdani7076 wrote:& anyone else,
Note the top of your model tree, that is not an assembly icon, it is a part/surface icon
.... it takes you into the Fusion software.
Frustrated and still hoping for a solution,
I don't use Fusion (change that in Application Options).
One extra step to push out the individual solids and assembly.
Lt. Rusty,
My apologies to you.
Just getting a bit frustrated. Trying to work as well as monitoring this
dilemma for our dept. I 'm hoping someonelse will eventually understand what going on here.
I've also forwarded this thread on to our reseller / support. Hoping they'll get involved as well
or point me in the right direction.
Thanks
Mark E.
For my problem:
after open the file -> export to *.sat
Open the *.sat file
It worked almost fine for what i needed
brunobpereira,
Thanks for the *sat workaround.
I tried your suggestion and I'm getting a good result.
The part labeling isn't quite what I'd like to see, so I'm guessing that would
be what you meant when you said your getting Almost everything you want.
For now this is OK and we can continue to work, although I still believe there must be an issue with the translator.
I'm not happy that I have to take the extra steps to get where we need to be.
I will continue to request an answer to Autodesk and this forum until I / we who use are not developers, but
users who sit at it 9 / 10 hours a day and know what is should be doing when its not doing it.
Thanks again.
P.S.. Those who are reading these, don't dismiss this and accept it as a solution.
Even though it works, its still not functioning the correct way.
Mark E.
Hi Mark,
I got your STEP file posted in message 6. This STEP file is clearly not an assembly. It has a single "shape" with multiple bodies. Inventor 2013 is doing correct to generate a part.
You can convert this part to an assembly using tool Manage->Layout->MakeComponents, Make sure the bodies are all selected from the Solid Bodies folder.
You are correct that Inventor2013 has removed the old button for "convert MSB to assembly" which was a workaround for old Inventor didn't allow multiple bodies in a part file. Now the translator does the correct job to convert a part to a part.
I am sorry for inconvenience if you always expected a STEP part with MSB to become an assembly in Inventor. Hope the MakeComponents still do the same job for you.
Let me know if you need the Inventor Assembly file that I created using MakeComponents.
Best Regards
Toni Qin
Platform Translation Team, Tech Lead
Autodesk Inc.