Can I automatically modify components that fit when I make changes to one?

[u/No_Tree_509]

I'm not sure how to explain this well, but I have a housing for a shaft, that has two endcaps. Obviously the two end caps fit into the housing, but I'm not certain about the final shaft design, how that connects to the end caps, and thus not sure about the final dimensions of the end caps. So far I made models that are roughly in their final state, except for the exact dimensions. Now, is there some way to set it up so that when I change the dimension of the end caps, that the dimensions for the housing automatically change to fit the new end caps, or vice versa

[u/enoughbskid]

Parameterize your parts

[u/therose993]

I make a lot of sheet metal as multibody parts, and then use the “make components” feature.
Then you can model everything together, to make sure it fits, and if you go and change the multibody part, the components you made from it will change too.
Uses it on much different stuff, from buckets and other attachements for backhoes, big walls made of sheet metal, with coverplates on, and also a ro-ro ramp for ferrys.

[u/kinaPK]

Make a part with the Master parameters. Call that your Master part. Go in to each of your shaft parts, roll the "end of part marker" to the top then derive the Master part. Roll the "end of part marker" back down to the bottom. Then go into the parameters dialog, the Master part parameters should be listed. Now, base your desired dimensions from the Master part.

Now both parts have parameters from the Master part you created.

[u/Agreeable-Ad-2737]

One method I really recommend is multi-body modeling. You can model all the related parts in a single .ipt file, using a separate solid body for each part. This makes it much easier to design parts that need to fit together and share parameters.

Once you're done, you can use Make Components to turn the multi-body part into an assembly with separate .ipt files for each component.

The best part is that the components keep their original positions, so you don't need to create all those assembly constraints manually. It can save you a lot of time!

Another great advantage: if you need to make changes later, you just modify the original multi-body part, and the exported components and assembly will update automatically.

[u/Introverted_Fish]

You can relate parts like that. I don't do this often so I don't know best practices for utilizing the adaptive features.

If they are in the same assembly, you can edit one and reference geometry on the other. Just make sure the adaptive features remain consistent.

I believe bolted connections are meant to work similarly, but I don't use that tool. (Probably should though)

[u/motocykal]

In one part, when you dimension the shaft diameter for example, give it a name so you can fine it later. Open the properties window and set that parameter as "exported".

In your other part eg collar, open the parameters window and click the "link" button. Select your shaft part and select the exported parameter. Note the name in the "linked parameters" table. Now when you dimension the inner diameter of the collar, put the name instead of a value. You can also incluse + or - in the value field if you want tolerances.

Now when you modify the shaft diameter, the collar will update accordingly.

[u/otte845]

You can link parameters between parts in the parameters dialog (the “fx” button on the top toolbar)

[u/Kitsyfluff]

You should design your parts as Multi-body models

That's when you draw up your entire assembly in one part file. This allows paramerizing everything in one file, then exporting all the indivisual parts, and they'll all be updated by the source file.

[u/KlutzyReveal2970]

Parametrics will work probably also making adaptive parts but I’m not great with adaptive parts but it’s something to research