Part features not shown in assembly modeling browser

[Anonymous]

Hello. I realy need help on this one.

I'm working in Inventor 2019 on a windows 10 machine, as a single user.

I work with iParts and iAssemblies.

When i place a part in the assembly, The modeling browser does not show my part features.

Several parts have patterns that I need to use in my assemblies. I think you all guesed allready. When I want to pattern a part, I can not select the pattern feature.

Below I have placed the feature tree of the part and the browser from the assembly. 

Any help is appreceated

[johnsonshiue]

Hi! The first image shows the iPart factory ipt file. The second image is the iPart member ipt file. The iPart member ipt file is a derived part of iPart factory ipt file with a table.

Could you tell me what you are trying to do with the iPart member file in the assembly?

Many thanks!

[Anonymous]

Hello Johnson.

Thanks for your reply.

In the iPart, I have a pattern.

I want to use this pattern to pattern parts in the assembly. In this case I need to make a bolted connection pattern.

At this moment, the iPart has only one item, but there will be more rows added in the table.

I hope You can help me out.

Kind regards:

Gerard de Vrught

[johnsonshiue]

Hi Gerad,

Unfortunately, I don't think the workflow will work. The iPart member does not carry the pattern feature data enabling the assembly to create the component pattern.

Unless you place the iPart factory inside the assembly (which you cannot do except converting a regular part to an iPart factory), you will need to pattern the component separately.

Many thanks!

[Anonymous · Accepted solution]

Hi Johnson.

Thanks a lot for your effort to help.

Too bad that what I wanted is not possible. It will give a lot of extra work.

Again. Thanks a lot.

Kind regards>

Gerard

[johnsonshiue]

Hi! iParts were designed to be standalone and self-contained library components. It was not meant to establish inter-component dependency.  One workflow you may consider is to publish the iPart as a Content Center part. The nice thing about this workflow is that, you retain the table definition. But, the part can be placed according to the selected configuration. Also, the features are still in the Content Center part.

Many thanks!

[JamieVJohnson2]

I would like add to this discussion, if you edit the iPart Table, you can add features and workpoints to the generated iParts with the FeatureName[Include] add to table option.  It creates a table column, and then generates the part with that feature in its browser tree.

[kerem.izmirli]

I am having the same issue, even though I'm not using an iPart, I just have a normal part file which has been derived into an assembly via "Make Component".

I have a top level assembly with two sub-assemblies, top level is an arrangement, one of the lower levels is existing concrete and the other sub is the new steel. I create everything in one master part and then derive out into their own assemblies/weldments. I have created a hole pattern using "Sketch Drive Pattern" in the master part to create holes in the concrete, but when I try to use "Associative Pattern" in the arrangement assembly level, I don't see any of my part features in my Assembly -> Modelling Tab.

Any assistance or explanation on what I'm doing wrong, or does the Associative pattern not work with sketch driven patterns?

Thank you in advance for any assistance 🙂

Regards, Kerem

[johnsonshiue]

Hi! This is not a supported workflow when you try driving the component pattern using a derived part. The derived part inherit the body geometry but not the feature recipes (only holes and threads can be passed down).

In your case, you will need to leverage Model States or make a copy of the original part (instead of deriving). The driving patterned feature must exist in the part.

Many thanks!

[kerem.izmirli]

Hi @johnsonshiue,

Thank you for your response!

Does using the "Make Component" feature on a solid treat the created part as a derived part?

Standard modelling practice in our office is multi-solid body part files which are exported into their corresponding weldments/sub-assemblies using "Make Component". Then I take all these sub-assemblies, and place them into another assembly which acts as the Top Level "Arrangement" assembly.

Is it possible to get this to work with my workflow?

Thank you advance for your responses 🙂

Kind Regards,

Kerem

[johnsonshiue]

Hi Kerem,

Yes, Make Components is like a combo command facilitating the Derive Part process. I guess you would still want the features, not just the body geometry. In that case, you may want to save the part as a different name. And use the new part. However, the two parts will not be linked. They become two independent parts.

Many thanks!