driving dimensions from other parts in an assembly

tnik wrote in news:48454ea7$0$20167 $ snipped-for-privacy@roadrunner.com:

Try designing the parts around a layout sketch in the assembly.

See; Help File\Layout sketches in assemblies (sw07)

rod

There are some interesting things you can do with in-context features. Suppose you have a dimension in a part that is driven by the distance between two unrelated other parts in an assembly. You want the dimension in the part to follow that assembly distance.

And we will assume that you can't just create an in-context reference in place to drive the part.

In the part:

1. Mate it in the assembly as needed.
2. Edit the part in the assembly.
3. Create a 3D sketch in the part.
4. Create a 3D line between the two driving parts in the assembly.
5. Place a dimension on the line. (It will be driven)
6. Create an equation in the part using the dimension from the 3D line to drive the dimension on the part.
7. Go back to assembly mode and change things; then do a CTRL - Q a couple times to check.

As a general rule you can use a side sketch as a kind of variable holder and have as many lines with dimensions as you want. This is how Ship In a Bottle works.

TOP

You can also use the equations in the assembly.

Deepak