Use parameter from assembly in a part

Forum|Forum|11 years ago
October 25, 2014
27 replies
18745 views

I created a parameter in my assembly and now I want to be able to use the value from that parameter in on of my assembled parts. But I can't figure out how to link that parameter to my part.

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Assembly Design

Best answer by ptc-5471878

I thought of a way to do this.

In the assembly I activate the part and start a sketch. In the sketch I reference the two axis in my main assembly that is the pitch and draw a line between them. Then I put a reference dimension on it. Exit the sketch and then create a new "pitch" parameter and then setup a relation that sets the new "pitch" parameter in the part equal to the reference dimension.

Now when I change the pitch parameter in the assembly, the pitch parameter in the part updates!

Happy days.

T

TomD.inPDX

17-Peridot

I am no expert at creating cross part references but I do know of a few options depending on what you are trying to achieve.

1st of all, you can easily create external references by activating a component in the assembly and using assembly references in the currently active part. I don't know the limitations, but take a sketch, for instance, and create assembly references in the sketch. These work well and they create an external reference automatically.

2nd, consider a flexible model in the assembly (make flexible). You can change a part feature to some assembly level value. There are quite a few options when you do this.

3rd, you can use merge models in case you need some extensive external reference. Typical for tooling operations, but useful in some other cases.

Things to remember about external references is to know when the part level updates and how changes are rolled up at all levels. This is where I get squeamish about external references. The more complex the operation, the higher the likelihood of corruption.

Can you share more about what you wish to achieve to better match a method?

P

ptc-5471878

Author

1-Visitor

I've attached a simplified assembly of what I am working on. I am designing a mold.

If you look at the attached picture there are parts that get bolted to the plate. I created the holes in the part first and then used them as a reference to create the holes in the plate.

I created a parameter called pitch to define where the parts are located. Now I want to use this pitch parameter to pattern the bolt holes in the plate using a relation.

Hopefully this makes sense.

2_example.zip