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How to handle multiple materials on one part

Phillip_BPhillip_B Member Posts: 26 PRO
In the plastics sector, it happens that a part consists of several materials:
- Hard component with molded soft component (different geometry areas)
- Base polymer and masterbatch (material compound)

How do you manage these scenarios in Onshape? Hard component and soft component could be managed as separate parts. However, these would then have to have a common part number and not be considered separately. When it comes to material compounds, I currently have no idea.

Background:
The materials used are relevant for compliance and must be traceable.

I am grateful for suggestions! :)

Comments

  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 4,368
    Composite Part (open) is what you need - the resultant composite part can then have 1 part num.
    Director, Technical Services, EMEAI
  • Phillip_BPhillip_B Member Posts: 26 PRO
    Composite part is a good tip! Thanks!
    It would be nice if you could see the individual materials in the BOM (i.e. several lines for the composite part).

    But what cannot be solved with this is the issue with the compound parts. Theoretically, several materials would have to be defined for one part and also output in several lines in the BOM.

    qty    name    material
    ...
    1       pump       material 1
                             material 2
                             material 3
    4       screw      material
    1       housing   material
    ...


    Does anyone have an idea?
  • Phillip_BPhillip_B Member Posts: 26 PRO
    Another point:
    When I check the mass of a composite part I get the correct result.
    If I insert the composite part into an assembly and check the mass there, it is also displayed correctly.
    However, if I want to output the mass in the BOM, only "no value" is displayed there.
    Did someone know how to get the mass into the BOM?
  • tim_hess427tim_hess427 Member Posts: 648 PRO
    I've treated overmolded parts as assemblies. That way, I can define part numbers for the individual components as well as the finished part and assign materials to each. A structured BOM could then show the individual components and materials. 

    Maybe you can get creative about having an assembly and composite part depending on your needs?
  • S1monS1mon Member Posts: 982 PRO
    I would also echo that an assembly can be more flexible and useful depending on your needs. Despite the fact that you may never ship the first shot of a double-shot or insert molded part to an end customer, you may want to get that "part" inspected or tested by itself in some way. It can be useful to track the materials, part numbering, etc as if it's a real part.

    That said, I've definitely done this the other way (multi-body as a single part) in Solidworks some times. It really depended on the project and the needs of how we wanted to manage the BOM and drawings.

    A part which has multiple materials is an "inseparable assembly". It could be a multi-shot injection molding, a weldment, a PCBA, sheetmetal with PEMs, etc... If there are parts which make up the inseparable assembly which might be shipped from one sub-supplier to another, then it makes a lot of sense to use an assembly and have part numbers for each piece. If all the assembly happens in one place, especially from raw materials, it could make more sense to use a single composite part. It really depends on what you need to order, track, inspect, etc. Also keep in mind repairs, refurbishment, CAPAs (corrective and protective actions), etc.
  • Phillip_BPhillip_B Member Posts: 26 PRO
    Thank you for the feedback. I will probably have to handle the parts individually. I was hoping for a unified path.

    Unfortunately, I can't solve the problem with the mass not being displayed in the BOM for composite parts. Does anyone have any ideas?


  • Phillip_BPhillip_B Member Posts: 26 PRO
    I created a support ticket for this and wanted to share the feedback here with you in case others are facing the same problem:

    I did some testing and the issues you are seeing are caused by a current limitation with how the Computed mass property is calculated when using composite parts.
    If you define a material for the parts that are components of a Composite part, the Mass properties tool will report the mass of this Composite part as the sum of the masses of the component parts of the Composite part.
    However, a Computed mass property will not be calculated for the Composite part itself. Hence, the Mass column in the BOM will not report the mass of the Composite part nor the Properties dialog of the Composite part will report a Computed mass property.

    There is an improvement request for this and I have added you to it.
    To work around this issue, you have a couple options:

    1.    Define a material for the Composite part. This will effective override the previous mass calculation of this Composite part (the sum of the masses of the component parts) and define a mass based on the material assigned to the Composite part.
    The computed mass property of this Composite part will also be calculated based on the assigned material and reported in the BOM.
    I would recommend you to do this if the material of all the components of the Composite parts is the same.
    The computed mass property of this Composite part will also be calculated based on the assigned material and reported in the BOM.
    I would recommend you to do this if the material of all the components of the Composite parts is the same.

    2.   
    Override the Computed mass property value of the Composite part on the Properties dialog and manually assign the sum of the masses of all component parts.
    The main disadvantage of this method is that you will have to manually update this override value if the mass of the component parts changes.

    Unfortunately, redefining the Composite part as a Subassembly will yield similar results since computed properties are not yet available for assemblies. I will add you to this other improvement request on a separate ticket.


  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,835 PRO
    While you're fixing composites, I'd like to retain the individual face colors also. Composites are great, but they don't look good.


  • eric_pestyeric_pesty Member Posts: 417 PRO
    billy2 said:
    While you're fixing composites, I'd like to retain the individual face colors also. Composites are great, but they don't look good.


    Appearances attached to actual faces are retained in closed composites (but not "part" appearances). I'm not sure what the underlying reasoning is for the different behavior between open and closed composite. It would be nice if you had a "toggle" in the composite appearance to keep existing appearances...
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,835 PRO
    edited February 28
    @eric_pesty I might be working to hard to make my models look real.

    I think retaining their colors would be nice. You can always add surface colors as an additional step. A lot of my composite parts are huge and re-colorizing them after composing, it's a lot of work.
  • eric_pestyeric_pesty Member Posts: 417 PRO
    billy2 said:
    @eric_pesty I might be working to hard to make my models look real.

    I think retaining their colors would be nice. You can always add surface colors as an additional step. A lot of my composite parts are huge and re-colorizing them after composing, it's a lot of work.
    I guess it depends on your workflow but if you know you are going to create a composite, you can assign colors to your part faces instead of the part itself as you create them (just box select the whole part and right click "add appearance to x faces"), which isn't really more work at the time, then they will be retained without needing to do anything else. Having to go back and do that would be fairly time consuming...

    Either way I agree more control would be nice, incidentally if you haven't use the "part color" custom feature, it doesn't solve your problem but it's pretty handy, especially if you want to configure colors!
    https://cad.onshape.com/documents/d997b0ffc30f659113b10c00/v/f17c7778c244710b6817a021/e/b6db0c9545b9a2df1d7ea546?jumpToIndex=828&showReturnToWorkspaceLink=true

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