BOM Items

GWS50

I would like to be able to group/configure columns so that items with the same name will show as 1 row and have a multiple number in the quantity column. I realise the the workflow is to only use a single item and duplicate in an assembly but sometimes when there are a few of the same parts in a part studio it can be easier to assemble them by inserting and them grouping them rather than have to use replicate (which is not always appropriate) of copy and mate.
For instances I have been using Igus bearings on a part studio which need to be dotted around the part studio so that the related parts can be drawn. Instead of inserting the bearings where they were drawn and grouping I am inserting one, copying and mating several times or, where appropriate, replicating.
I hope this makes senses!

PeteYodis

@GWS50 Are you essentially wanting specific IGUS bushings wherever you have certain holes that those would be installed into?  I think there are other ways to efficiently get what you want, rather than hacking the assembly BOM this way.  

GWS50

Yes I guess that's right. I think that perhaps using the transform with mate connectors would be a good way of populating the bushings in a part studio but would that work in the BOM?

GWS50

Actually the transform tool is what I used to populate.
Not sure how I can drop parts into an assembly with the same name so they only show in one row in the BOM.

GWS50

PeteYodis said:

@GWS50 Are you essentially wanting specific IGUS bushings wherever you have certain holes that those would be installed into?  I think there are other ways to efficiently get what you want, rather than hacking the assembly BOM this way.  

Pete, could you elaborate a little please how the workflow

tim_hess427

@GWS50 - I think what Pete was alluding to is that it sounds like you might be better served using an in-context part studio. If you copy a part in a part studio, the copies will have different internal ID's, so if you insert all of them into the Assembly, Onshape has no way of knowing that they should be grouped together. 

To back up a bit, it sounds like what you're doing is creating multiple bushings in your part studio, and then modeling around them. Then, you when you get to your assembly, do don't want to go through the hassle of placing/mating all of your bushings a second time. This, I think is a fairly common issue with a couple of solutions. (Excuse me, if this assessment is not accurate). 

One solution is to use in-context editing, where you have a single bushing model, and insert that same model into the assembly as many times as needed. You can also create a layout sketch to help position the bushings when inserting them into the assembly. Arrange the bushings as necessary, then create an in-context part studio to design parts around them. 

Alternatively, you could model a "dummy solid" in your part studio that has your bushing dimensions. Then, you can use the transform tool or Point Pattern feature script to place the dummy model where you want your bushings. Finally, use a boolean operation to subtract the dummy solid from your part. That said, the in-context part studio workflow is probably a little more efficient. 

GWS50

Thanks Tim, your assessment is correct!
I'm not sure how the in-context would help as it sounds like I still need to insert the bushing into the assembly multiple times. I think I must be misunderstanding your solution. I don't use in-context editing that much as I find it hard to keep track once you have more than one or two contexts to update.
I also can't see how the 'Dummy Solid' would help....perhaps I'm missing the point.
I'll have a look at the learning centre to try and gain some more knowledge.
Thank you for your time and explanation.

tim_hess427

@GWS50 - For the first option described - you insert the bushing into the assembly multiple times instead of inserting the bushing into the part studio. It'll be more efficient because you're not having to assemble the bushings in both tabs. An assembly tab is designed for this type of operation. When you insert the same bushing into an assembly multiple times, the BOM will correctly combine them into one line. So, with this option, you are only positioning the bushings once and the BOM will act you expect. 

I suspect scenarios like your are exactly why in-context editing was added. While part studios can contain multiple parts, they are not designed for creating assemblies and treat each body as being unique, even if the geometry is identical. 

The "dummy solid" option is just another way to get the correct bushing geometry into the part studio without actually bringing the bushings into the part studio. I agree with you in that I still don't feel completely comfortable with "in-context" part studios for some reason that I can't quite put my finger on. However, I think they're your best tool in this situation. 

Maybe someone else has other options?

GWS50

Ah right got you now, thank you for clearing that up and thank you for your patience. I will try a test project and see how it goes.
The In-context scenario seems hard to keep track of for some reason. When I have tried it in the past things have gone awry because of multiple 'In-context' parts and their corresponding updates. It's fine with just one in-context link though.