Saving assemblies as parts

claus_jeppesen817

Need to have

MBartlett21

@claus_jeppesen817
Please create an improvement request, or vote up an existing one in the category on the right

philip_thomas

@claus_jeppesen817 - I wonder if you be so kind as to take a moment and let me know what you're trying to do?

Are you trying to export a single file with the entire assembly?
Are you trying to export each part in the assembly as a separate part?
Are you trying to boolean all the parts together as a single body?

Please be very specific and clear and i will see what i can do to help you.

Many thanks - Philip.

MBartlett21

@philip_thomas

I had an assembly and wanted to export it as a Multi-Body part in Solidworks.
I had to create a part studio, copy all the parts in place, change their colour to match, then export it as a part.
I would like to shorten this workflow

claus_jeppesen817

philip_thomas said:

@claus_jeppesen817 - I wonder if you be so kind as to take a moment and let me know what you're trying to do?

Are you trying to export a single file with the entire assembly?
Are you trying to export each part in the assembly as a separate part?
Are you trying to boolean all the parts together as a single body?

Please be very specific and clear and i will see what i can do to help you.

Many thanks - Philip.

1) If I download a component (PLC, motor, bearing housing etc) it is often an assy. I want to use it as a part. You can do that in Solid Works
2) In Onshape i have experienced that an imported STEP file is dissolved into  non constrained surfaces. It does not help to group them as all surfaces are shown in a BOM. How is this avoided?

philip_thomas

@claus_jeppesen817 - thank you for explaining what your goal was. 
There is an excellent technical paper in the learning center that describes setting up standard part libraries. 
Bottom line, you have some options. 
1)import the step assembly as ‘flattened’ (creates a single part studio with all instances. From here you can either (a) Boolean all parts to create alone part. Name the part and add meta data (pn etc). (B) insert the part studio into an assembly and apply a ‘group’ mate. Add meta data and you’re done. Version the document and now you have a standard part document that you can link into your designs. Do not add any other parts to the document as you will have to version it again - falsely notifiying all other users that the first part is out of date. 

@mbartlett21    Yes that is the simplest workflow - not sure why you need to change the colors, but just in case there is a reason, you know you can change the colors of all parts simultaneously?

The bigger question is why would you want to export an assembly as a multi-body part? 

MBartlett21

@philip_thomas

To use it like a single part in Solidworks

john_mcclary

philip_thomas said:

@claus_jeppesen817 - thank you for explaining what your goal was. 
There is an excellent technical paper in the learning center that describes setting up standard part libraries. 
Bottom line, you have some options. 
1)import the step assembly as ‘flattened’ (creates a single part studio with all instances. From here you can either (a) Boolean all parts to create alone part. Name the part and add meta data (pn etc). (B) insert the part studio into an assembly and apply a ‘group’ mate. Add meta data and you’re done. Version the document and now you have a standard part document that you can link into your designs. Do not add any other parts to the document as you will have to version it again - falsely notifiying all other users that the first part is out of date. 

@mbartlett21    Yes that is the simplest workflow - not sure why you need to change the colors, but just in case there is a reason, you know you can change the colors of all parts simultaneously?

The bigger question is why would you want to export an assembly as a multi-body part? 

Well said philip, those work flows have suited my fine while in Onshape

As for exporting an assembly as multi-body,
When we receive an assembly from a customer, or vendor. It is typically something that shouldn't be modified by us anyways.

We don't want to have a 10 part 1 assembly structure for every purchased part (ex: gearmotor)
So saving as a multibody part just makes the structure cleaner for somethings that don't need that level of complexity.

Another thing to note for those in Solidworks, After exporting as an assembly, you can open the assembly in Solidworks and set all the parts to "virtual", this will allow you to delete all of the extra parts in your folder as well, and you just treat the assembly as a multibody part. I do this for objects like pneumatic cylinders so I can have a single part in my tree, but still be able to animate strokes.

Another trick you can to in solidworks is open the assembly, then "save as" a .sldprt
This will create a multibody part.

Also: If you export your part studio as "Solidworks" it will save as a multibody as well.
This method is fewer steps, but can be very very slow for larger assemblies. (in fact today i tried 3 times to export a rack with one body panel and it took half hour or so and failed in the end) But for small 10 part or so I assume, these export quickly.

@claus_jeppesen817 : you can exclude items from a bom by checking the box in the part properties, or you can set the bom hierarchy to structured to hide all the sub-details.