Working with imported step file that results in a lot of part copies

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Hello,

 

I downloaded a step file from McMaster Carr for a needle bearing.  The file comes in with one base feature and a lot of part copies.  In the past, I was able to import the file into an assembly template and the sub-components would end up as part files.  How can I get all of the part copies efficiently into either their own part files or even as a single file?  I am attaching the part file from ST7 and the step file.  

 

Thanks,

 

Kyle

Kyle Joiner
IPA LLC
ST10 MP1
30 REPLIES

Re: Working with imported step file that results in a lot of part copies

Siemens Phenom Siemens Phenom
Siemens Phenom

Kyle,

Find the "Step3D.ini" file in your Program folder (...Program Files/Solid Edge ST7/Program).

Edit into it and modify the line shown to "Off":

Step3DINI.JPGResult.JPG

Kevin Grayson
Solid Edge Technical Consultant
kevin.grayson@siemens.com

Re: Working with imported step file that results in a lot of part copies

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Kevin,

 

Wow, I would have never found that.  Thanks for the help!

 

What would be the advantage of leaving the setting on and letting the file come in as multiple bodies?  Is there a way to work with it is multiple bodies?

 

Kyle

Kyle Joiner
IPA LLC
ST10 MP1

Re: Working with imported step file that results in a lot of part copies

Siemens Phenom Siemens Phenom
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Kyle,

You could open it with the settings "as is" and let it come in as multi-body.  Another option to publish multiple files would be to use the "Multi-Body Publish" command which would write out individual part files.  Assuming you wouldn't need to modify this part since it's from MMC.  However, if you wanted to modify it, the published assembly (result of "Multi-Body Publish") is linked back to the original multi-body file.  You could edit that "part" and those changes translate to the published assembly.

 

Hope this helps.

Kevin Grayson
Solid Edge Technical Consultant
kevin.grayson@siemens.com

Re: Working with imported step file that results in a lot of part copies

Phenom
Phenom

Kevin,

 

As I'm sure you'll agree, the need to "EDIT" an "ini" file in this day and age just to properly import a model is one of the worse experiences I have with Solid Edge.

 

Like Kyle, I often download vendor parts and we are all guessing as to how they've saved them in their exported format. So with SE the user is stuck wasting an enormous amount of time fiddling with "ini" files, just to do something that should be really fast and easy.... it's almost 2015!

 

Anyway the whole concept of using "imported" Parts is to SAVE the user TIME and aggravation.... in fact Solid Edge brags about this capability. But as Kyles exercise proves, it can't even handle the simplest of imports without a bit of torture.

 

I now model simple parts like bearings from McMaster Carr faster then I can import them... tells you something is wrong!

 

Bob

Re: Working with imported step file that results in a lot of part copies

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Phenom

100% agree Bob. The exclusion of these options from the...um....Options box!!..... and their banishment to the .ini file is baffling.

-Dylan Gondyke

Re: Working with imported step file that results in a lot of part copies

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Hi Kevin,

 

In my system, the multi body publish option was grayed out.  I have to admit I'm a complete novice with multi body.  I frequently used he split part command on earlier versions.  I'll explore multi body more when I encounter a situation that requires it.

 

Kyle

Kyle Joiner
IPA LLC
ST10 MP1

Re: Working with imported step file that results in a lot of part copies

Siemens Phenom Siemens Phenom
Siemens Phenom

Kyle,

That's strange.  When you open the STEP file, does your Pathfinder look like this?:

 

MB.jpg

 

You have to save the multi-body "par" file before it will let you publish but even still the command shouldn't be grayed out (assuming you have Foundation, Classic, or Premium).

 

On a side note, multi-body is handy for different scenarios:

1) Your case where you download/import a "part" file that has several bodies in it and you need them as individual part files.  Use Multi-Body Publish.

2) You want to bring in an "assembly" file but have it represented in your BOM as a single "part".  Allows you to open assemblies into part as multi-body.

3) Conceptual design tool:  Instead of using Create-in-Place in assembly and creating multiple files on disk, open a single Part template and create all your "parts" by using "Add Body".  The benefit of this method is that the power of synchronous tools can be used across multiple bodies at the same time as you're tweaking your conceptual design.  You don't have to worry up front about assembly constraints, etc as you edit.

 

I'm sure there are others but these are the ones I think of.

 

Hope this helps.

 

Kevin

Kevin Grayson
Solid Edge Technical Consultant
kevin.grayson@siemens.com

Re: Working with imported step file that results in a lot of part copies

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Hi Grayson,

 

I overwrote the original file with the new one after you showed me the .ini edit so I don't have it anymore.  Basically, my file imported with a base feature and a bunch of part copies but it did not have the solid bodies listed in the tree as yours does.  I did import my into an ordered file whereas it looks like your file is set for synchronous so I don't know if that has any effect.

 

Kyle

Kyle Joiner
IPA LLC
ST10 MP1

Re: Working with imported step file that results in a lot of part copies

Phenom
Phenom

Kyle, if you do mess with these, it's good practice to first copy and rename the original .ini file, to something like STEP3DOLD.ini. This way, you can easily swap back to the unmolested file if you get yourself in trouble with options changes. 

-Dylan Gondyke