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Creating a part with multiple material layers

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Creating a part with multiple material layers


I am looking to create a part in Creo that represents a metallised plastic part. The base material is made from a plastic material and it has a very thin (10um) copper layer on top of the plastic with a final nickel layer (5um) on top of the copper.

Is there a way of applying these additional layers of material onto the surface of the existing part?

I intend to carry out some stress analysis on the part if I can achieve this build up of layers in the model.

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Creating a part with multiple material layers

It is always best to do something before trying to give advice on how to do it

I had the opportunity to try this and the results were good.

The best part of the attached assembly is that it remains parametric; the worst part of the attached assembly is that it remains parametric.

What that means to say is that you have levels of dependency where any one failure will fail everything. Nothing new here.

Note that the plastic part here is 50mm x 50mm x 20mm. This is important to know when relative accuracy becomes an issue.

At 10um (0.01mm), the offset and merge worked fine. At 5um (0.005mm), the relative accuracy required an adjustment to .0001 (something less than .0012 default).

If I change the plastic part, the clad models change with it, as long as the offsets and cut-outs (merge) features remain viable.

Attached is a full version Creo 2.0 assembly to explore.

Note the feature order explained below the image.

composite_assembly.PNG

The assembly has the master plastic part assembled.

PRT0609 was added with just CS0 and the default datums (model set to MM)

PRT0609 was Activated and under the Get Data drop-down, you have Merge/Inheritance active. Select this feature.

Select PRT0608 to merge into PRT0609

Open PRT0609 and create a solid offset to the inner surfaces. This takes some knowing, but use the filter (geometry) and select through until you get the "intent surface". Pick all applicable surfaces.

Use offset, and select the non-tapered solid offset option.

Go back to the assembly and activate PRT0609 again.

Again merge PRT0608 but this time use the "remove material" option in the merge dialog.

What remains is the clad solid.

Do the same with PRT0610 only use PRT0609 instead of the plastic master, PRT0608.

Hint: to make offset selection easier for PRT0610, use a larger offset in PRT0609 for the time being. I used 0.5 so I could tell what I was selecting; inside or outside. Once you are done, you can set PRT0609 back to 0.01 and PRT0610 will follow on a regen.

19 REPLIES 19

Re: Creating a part with multiple material layers

You are describing an assembly of different materials; there's not an option to have a part do this.

Re: Creating a part with multiple material layers

Hello, Calum

Your thicknesses are so small that I do not know if Creo will see.

I think we will have to increase the accuracy of your parts to its maximum, have you ever tried.

Now is what these thin layers will really significantly change the characteristics of your parts.

Best Regards.

Denis.

Re: Creating a part with multiple material layers

Yes, you will need to set the accuracy significantly higher... maybe set it to absolute depending on the part size.

To have different materials, you will need some kind of assembly. That is the only way you can have analysis recognize the different properties.

There are several ways to accomplish the clad models.

As an aside, can you share references of who can do this plating and the kinds of plastics are conducive to the process?

Re: Creating a part with multiple material layers

Yes but I am still unsure as to how I can create an assembly with different layers on the part?

Re: Creating a part with multiple material layers

I have set my accuracy to the best that Creo can achieve but I am not sure how to apply the additional material surfaces that I mentioned in my original query.

Re: Creating a part with multiple material layers

It depends on what type of plating that you wish to use and what the intended prupose of the part is for. There are several companies in the UK who can coat a range of plastic materials from ABS to PEEK-type materials.

Re: Creating a part with multiple material layers

Copper/Nickel is a good EMI/EMC material. That is what peeked my interest. Can you link me to one of these suppliers?

As the how; you might look into the Merge functionality if you wish to remain somewhat parametric.

The easy solution is Offset of the surface making it a solid bigger than the original and then subtracting the original from the merge.

Merge is the Creo equivalent of Boolean operations but it has to be done with outside references.

If you care to post a test part, we can see what it takes to do this in Creo.

Use the advanced editor to attach files.

Re: Creating a part with multiple material layers

You should look at the analysis software for options. It's more likely that you'll need shell elements to handle this; all that will come from the solid will be bricks or tet elements and they will either be highly distorted or very small.

Re: Creating a part with multiple material layers

It is always best to do something before trying to give advice on how to do it

I had the opportunity to try this and the results were good.

The best part of the attached assembly is that it remains parametric; the worst part of the attached assembly is that it remains parametric.

What that means to say is that you have levels of dependency where any one failure will fail everything. Nothing new here.

Note that the plastic part here is 50mm x 50mm x 20mm. This is important to know when relative accuracy becomes an issue.

At 10um (0.01mm), the offset and merge worked fine. At 5um (0.005mm), the relative accuracy required an adjustment to .0001 (something less than .0012 default).

If I change the plastic part, the clad models change with it, as long as the offsets and cut-outs (merge) features remain viable.

Attached is a full version Creo 2.0 assembly to explore.

Note the feature order explained below the image.

composite_assembly.PNG

The assembly has the master plastic part assembled.

PRT0609 was added with just CS0 and the default datums (model set to MM)

PRT0609 was Activated and under the Get Data drop-down, you have Merge/Inheritance active. Select this feature.

Select PRT0608 to merge into PRT0609

Open PRT0609 and create a solid offset to the inner surfaces. This takes some knowing, but use the filter (geometry) and select through until you get the "intent surface". Pick all applicable surfaces.

Use offset, and select the non-tapered solid offset option.

Go back to the assembly and activate PRT0609 again.

Again merge PRT0608 but this time use the "remove material" option in the merge dialog.

What remains is the clad solid.

Do the same with PRT0610 only use PRT0609 instead of the plastic master, PRT0608.

Hint: to make offset selection easier for PRT0610, use a larger offset in PRT0609 for the time being. I used 0.5 so I could tell what I was selecting; inside or outside. Once you are done, you can set PRT0609 back to 0.01 and PRT0610 will follow on a regen.