Sketch Won't Update with User Parameters

[Tibblesworth]

Hello all,

I'm very new to Fusion 360 so hopefully my issue is something an experienced eye can catch quickly.

The problem I'm having is with rotating a copy+pasted sketch about the Z-axis based on user defined parameters. I can set the sketch rotation once upon its creation using said parameters, but if I update the parameters afterwards, the sketch rotation does not change.

My trouble shooting of this issue has involved the following work flow:

The sketch above is copy+pasted from the one below. Rotation is not yet applied.

Top-Down View: The "Move" command is set up like so, rotation of Sketch Objects about the Z-axis applied using user defined parameters.

Move command is completed, but does not show up in the design timeline. Updating the User Parameters does not change rotation the angle after creation.

I'm assuming there's a much easier way to go about this and any input would be greatly appreciated.

Happy Holidays

[jeff_strater · Accepted solution]

Sketch Move does not create a timeline feature, and is not expected to.  Moves within a sketch are applied to geometry within the sketch.  There is no history within a sketch.  There are a couple of ways to do what you want to do, I think.  One is to create a component for the sketch, and use component instances of that component. with joints between them to control the rotation of instances.  The second would be to fully define your sketch with dimensions and constraints, then have a user parameter tied to an angle dimension to control the rotation.

[g-andresen]

Hi,

If we know what is to be achieved in the end, we can make an informed statement.
This would require a picture of a (similar) real existing object and an insight into the current design (f3d file).

Please share the file.

File > export > save as f3d on local drive  > attach it to the next post.

günther

[Tibblesworth]

Ah ha!

Joints, what a great idea. I can confirm that sketch does update when User Parameters are changed, so I believe I will go down this path. I'm coming from a different CAD software package and my workflow generally doesn't involve using mates/joints until much later.

For those who have the same issue, I did the following:

Copy Original Sketch

Assemble --> New Component -->  Activate is checked  -->Ok

Create Sketch --> Paste

Activate Original Component

Assemble --> Joint --> Component 1 --> Select any part of the new sketch (I chose a concentric circle)

--> Component 2 --> Select the Origin (assuming you've used the origin as a basis for your design)

Enter your Angle and/or Offset using User Parameters and they should update as expected --> Ok

Now, I'm troubleshooting some odd issues while using the "Thicken" command on surfaces generated via Loft between the two sketches. The "thickened" bodies appear at the original, non-rotated, angle. However, given some time I should figure it out. Never-mind, it seemed to be a timeline related issue. Once I deleted the old loft command and made a new one with the same settings, it executed the proper rotation.

Thank you for your help!