Inserting derived assembly into part studio

gerald_friedman

There are parts I've downloaded that are assemblies; bearings for example that have inner and outer races, retainers, and balls.
When I attempt to insert the bearing as a derived part into a part studio I'm working in it comes in as individual parts.
There doesn't appear to be a way to group the individual parts once inserted so it's difficult to relocate to the desired position.
Any thoughts?

gerald_friedman

Works!

Quote Philip:

"Another method would to import the bearing into a part studio and extrude a cylinder with a (larger) hole through the thickness of the bearing to merge the balls, inner and outer races into a single part. This method is less work up front, but means that you won't see the individual bearings in the assembly (although on the plus side, a bearing becomes a single part number)."

Very helpful.

gerry

3dcad

Have you checked option 'flatten' during import?

Or you can use another format that imports as single part if that's what you wan't.

gerald_friedman

I've tried Step and Iges and flattening.

Neither work.

I'll try some other formats.

gerald_friedman

Well, tried SAT and Solidworks and both also failed.

All arrive as individual component parts.

coleman

You can group the parts after they are inserted.  Drag a bounding box around the parts to select them and click group.  

I group parts like that when I don't need to have motion mates. 

On components like pneumatic air cylinders where I do need to simulate the motion....I create a sub-assembly first and then bring that into the main assembly. 

gerald_friedman

There is no GROUP in a part studio that I can find.

Only in an assembly.

I'm pulling a derived part into a Part Studio where I'm doing all the design work.

philip_thomas

This is a classic problem in CAD. No data format will change the way the parts are treated, a part is a part.
When importing, your choices are to import as multiple parts into a part studio or as an assembly.
This is the intended behaviour.

If imported as an assembly, the group command saves you a ton of work when importing into other assemblies.

If you wish to derive into a part studio (to size other parts), then things get a little more involved. In the case of a bearing, I personally would make a cylinder with a hole in it to represent the physical size and build the parts off that.

Another method would to import the bearing into a part studio and extrude a cylinder with a (larger) hole through the thickness of the bearing to merge the balls, inner and outer races into a single part. This method is less work up front, but means that you won't see the individual bearings in the assembly (although on the plus side, a bearing becomes a single part number).

A part studio is not for assembling parts - that's what assemblies are for. That said, the workflow you describe is valid and hopefully the methodologies described here will help you. On our side, we are always looking at improving standard workflows and position parts within a part studio is one that we are looking at.

I hope this helps - Philip . . . 

peter_hall

I have a similar issue when I bring in clamps and need to work with them in a parts studio. I remake the important parts that I want to use in the parts studio,( a freaky looking clamp substitute ) then I build the rest of the fixture and substitute my freak clamp for the real downloaded clamp in my assembly.

gerald_friedman

Philip,

Understood. I'll try your advice.

Thanks,

gerry

philip_thomas

gerald_friedman said:

Philip,

Understood. I'll try your advice.

Thanks,

gerry

Gerald - please feel free to ask any question and yes, we are looking to make this easier moving forward - thank you.

gerald_friedman

Works!

Quote Philip:

"Another method would to import the bearing into a part studio and extrude a cylinder with a (larger) hole through the thickness of the bearing to merge the balls, inner and outer races into a single part. This method is less work up front, but means that you won't see the individual bearings in the assembly (although on the plus side, a bearing becomes a single part number)."

Very helpful.

gerry

murray_cox

Hi everyone, I realise this is an old thread, but I'm faced with exactly this issue.

I *frequently* pull complicated assemblies from other sources into my designs and create new parts to link them or attach to them, and I'm not sure if onshape can accommodate this workflow very well or if I'm missing something. An example - I want to design an enclosure around a raspberry pi. I find a great (assembly) model online with connector locations, mounting holes, etc. After import I have an assembly, which I can't then use as a 'derived' part in a part studio to act as a reference when designing the new parts to surround it. Another example - want to design a mounting bracket for a gearbox. A beautiful cad model of the gearbox is available - but as an assembly. Sometimes I can pull just the appropriate part (say the housing) from that assembly to use as a derived part in onshape, but it would be really good to have the entire assembly visible and ideally able to be referenced when designing a bracket to suit. 

Perhaps I need to 'flatten' the assembly into one part first, perhaps by an re-export/re-import process.

philip_thomas

@murray_cox - This is an important topic and worth a couple of mins.
There are several variations on this workflow, but the main premise is that i need to build a part that references one or more other parts in a specific orientations.
The classic workflow involves building parts, assembling them and then building a new part 'in context'. 
There are some problems with this workflow and while we fully intend to support it, but want to do it better than anyone has to this point.
There are two alternatives that exist within Onshape today.
(1) If a part studio contains a part that needs to be editing WRT a part in another part studio (or other document), the process is to derive the referenced part into the first part studio and then 'transform by mate connector' to position/orient it and then create the new feature.
(2) An imported assembly (via STEP/Parasolid) comes with an option to 'flatten' an assembly to a single part studio (along with an assembly). This now enables a new part to be built in the newly created part studio OR (as above) the ability to derive a part into another part studio (and saves the transform by mate connector because the part is already in the correct orientation).
I hope this helps and please feel free to ask any questions.

murray_cox

Hi everyone, I realise this is an old thread, but I'm faced with exactly this issue.

I *frequently* pull complicated assemblies from other sources into my designs, and I'm not sure if onshape can accommodate this workflow very well or if I'm missing something. An example - I want to design an enclosure around a raspberry pi. I find a great (assembly) model online with connector locations, mounting holes, etc. After import I have an assembly, which I can't then use as a 'derived' part in a part studio to act as a reference when designing the new parts to surround it.

Perhaps I need to re-export the assembly as a single merged part that can then be used in a part studio somehow?

Narayan_K

@ murray_cox  you can save assembly as step file then you can import it to Onshape part studio.

3dcad

You don't even need to save the file into your computer, just export with option 'Store file in new tab' and then import back with 'flatten' option checked. You will get all parts into same part studio.

In your case, you should do this to the original file grapped from web. Just use flatten when importing to Onshape and you can immediately use imported parts as reference to new ones.

murray_cox

Thanks @phillip_thomas, @3dcad and @Narayan_K, much appreciated.

I've just tried the approach of importing with 'flatten' option - and indeed I now get all the parts contained within one part studio. I can then use a derived version of that former assembly, now part in a new part studio.

Looks like I still need to learn about the 'transform by mate connector' functionality however. Although the derived part in the new part studio shows all the components of the original assembly, when I try to transform, I can only select one component and transform that, the rest stay where the original derive operation put them.

3dcad

You need to select all parts that you wan't to move. You can try to boolean unite all parts into one body in original part studio, if they touch each other and there is no 'zero manifold bodies' it should perform ok by box selecting whole model and boolean.
This way you would end up with single part to move after derive.

philip_thomas

@murray_cox - Transform by mate connector allows the selection of multiple parts.
You should be able to move all the 'assembly' components with one feature.

murray_cox

Yes! that seems to work, thanks.

A couple of oddities - it leaves the original position of the mate on the derived part ('assembly') visible in it's old position, but it can be hidden so it doesn't clutter things up, and also you need to select the components of the derived part/assembly in the transform by mate connector operation via dragging a selection region or individual clicking within the 3d design view as they are not individually listed in the hierarchy tree view (only summarised by the 'derived1' or whatever the derived collection of parts is called, which doesn't seem to be valid as a transform selection if clicked). That might cause some pain if the derive operation placed the part/assembly coincident with other existing parts, but the existing parts could always be hidden out of the way.

philip_thomas

@murray_cox - Yes, the orphan mate connector is a 'not quite a bug but clearly there is a better way" - this will be 'improved'

trampas_Stern

I am having same problem I need to import a step file into an existing part studio, to add mounts for the part in the step file. 

The mating connector does not work with the step file.  So far the only option I have found is to stop using onshape and go back to freecad. 

philip_thomas

@trampas_Stern - not that freeCAD isn't a fine installed CAD product, perhaps you could help us understand what you are struggling with?
To insert imported data into an existing part studio, you have a couple of options;

Option1
1) import the step file into a new document (with or without flattening)
2) Version the newly created document (needed in order to link to it)
3) DERIVE 1 or more parts from a named version of the new document into the part studio containing your existing data
4) Use transform-by-mate-connector to position/orient the newly derived parts

Option 2
1) import the step file into your existing document (with or without flattening)
2) DERIVE 1 or more parts from the newly created elements into the part studio containing your existing data
4) Use transform-by-mate-connector to position/orient the newly derived parts


I am happy to answer any questions - i hope this helps.

famadorian

Is there something new regarding this issue, cause I can't really see this solved or I didn't understand whatever conclusion was given here;)

I have a piece of land where I'm drawing roads and such in a part studio and I want to insert a house assembly. 

philip_thomas

@famadorian - we are trying to figure out how to help you.
Multiple suggestions have been made and at least one answer has been accepted.
What is it that you are still not able to do or are waiting for?
Thank you.

booshack

When inside the assembly, you can create a part studio in context. Then box select all the parts and copy in place with transform. Then select all those and make a composite part. This composite part can then be inserted in your other part studio with derived part