topic Re: Cannot edit circular pattern in a sketch in Fusion Support Forum

Cannot edit circular pattern in a sketch

Anonymous — Wed, 22 Sep 2021 10:47:00 GMT

After one of the latest updates, i cannot edit a circular pattern in a circle in a sketch anymore.

Is this the expected behavior.

I have been able to edit the pattern in this exact sketch before.

Re: Cannot edit circular pattern in a sketch

seth.madore — Wed, 22 Sep 2021 10:49:53 GMT

Could you share the file or a screencast demonstrating this behavior?

Re: Cannot edit circular pattern in a sketch

g-andresen — Wed, 22 Sep 2021 11:03:01 GMT

Hi,

works as expected, but perhaps the menu does not show all options.

günther

Re: Cannot edit circular pattern in a sketch

Anonymous — Wed, 22 Sep 2021 11:20:58 GMT

https://knowledge.autodesk.com/community/screencast/6073f1ef-9686-4319-a2c6-e05a9a2e8b58

Re: Cannot edit circular pattern in a sketch

Anonymous — Wed, 22 Sep 2021 11:26:14 GMT

If I make another circle and a pattern inside, I can edit that new pattern perfectly. Its the existing pattern from a loaded file I cannot edit.

Re: Cannot edit circular pattern in a sketch

davebYYPCU — Wed, 22 Sep 2021 11:30:56 GMT

Well not like that you can't.

Edit sketch.

Left click select the pattern Icon - highlights darker blue

right click and select Edit Pattern from the menu.

Might help....

Re: Cannot edit circular pattern in a sketch

Anonymous — Wed, 22 Sep 2021 11:33:33 GMT

None of that works, the parttern marker never goes dark.
Try this file. https://a360.co/2VZJVRU

Re: Cannot edit circular pattern in a sketch

davebYYPCU — Wed, 22 Sep 2021 11:43:24 GMT

No problem.

Might help.....

Re: Cannot edit circular pattern in a sketch

g-andresen — Wed, 22 Sep 2021 11:57:49 GMT

Hi,

I suspect that the command here is (uniquely) corrupt.
I can only strongly recommend that you create patterns not in the sketch but as a feature.
This way you always get the new current state when the quantities change and you don't have to execute the extrusion command manually after changing the sketch.

günther

Re: Cannot edit circular pattern in a sketch

TheCADWhisperer — Wed, 22 Sep 2021 12:29:23 GMT

@Anonymous wrote:
Its the existing pattern from a loaded file I cannot edit.

You are not using the most computationally efficient technique.

It is all wrong to pattern sketch elements like this.

As suggested by @g-andresen - pattern feature rather than sketch.

It would also be helpful if you Attach files here rather than link. (Faster on our end.)

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Re: Cannot edit circular pattern in a sketch

Anonymous — Wed, 22 Sep 2021 12:42:18 GMT

OK, I have found the problem. When you want to edit a circular pattern in a sketch, apparantly you need to mark the center of the pattern before you can hover the parttern icon to darken it.

But in the file I have, the circle has N points on top of each other, which makes it really hard to find the point enabling the pattern.

Re: Cannot edit circular pattern in a sketch

TheCADWhisperer — Wed, 22 Sep 2021 13:38:26 GMT

@Anonymous wrote:
... circular pattern in a sketch,

Not the correct technique for this design.

Re: Cannot edit circular pattern in a sketch

Anonymous — Wed, 22 Sep 2021 15:24:54 GMT

I redesigned with a different technique, using pattern outside the sketch. Now the recalculation is much faster and much more stable. But now I face the problem of having many bodies making it annoying to work with for export or 3D printing.

Having many bodies is also annoying in this case: I need a belt of 90 teeth and a belt of 200 teeth. First i make a belt of 90 teeth, combine all bodies and 3D print it. Then I change the number of teeth parameter to 200, but the combine does not add in the extra bodies so now I have a 90 tooth piece and then another 110 loose teeth 🙂

What is the best technique, if I need a single body as result after changing the number of teeth parameter.

If just the circular pattern dialog (outside sketch) could have the option of combining bodies that touch each other.

Re: Cannot edit circular pattern in a sketch

TheCADWhisperer — Wed, 22 Sep 2021 16:01:37 GMT

@Anonymous wrote:

But now I face the problem of having many bodies making it annoying to work with for export or 3D printing.

What is the best technique, if I need a single body as result after changing the number of teeth parameter.

Attach the new version here.

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

It is all in the order of operations and the Options you select when creating the pattern whether you get one body or multiple bodies.

Re: Cannot edit circular pattern in a sketch

g-andresen — Wed, 22 Sep 2021 17:16:20 GMT

Hi,

extrude one tooth on the belt with the JOIN option.
Then create a pattern (Type FEATURE) and select the last extrusion feature (tooth) from your timeline.

This way there is only 1 body.

günther

Re: Cannot edit circular pattern in a sketch

davebYYPCU — Wed, 22 Sep 2021 21:13:53 GMT

Change the timeline order of operations.

Make one tooth, pattern them.

Edits for count done here, before next step

create - Extrude / Sweep the “Band” with Join, will merge all teeth to one body.

Might help.....

Re: Cannot edit circular pattern in a sketch

Anonymous — Fri, 24 Sep 2021 08:03:00 GMT

Hi,

I've been busy with other suff, but here the new one is attached.

Re: Cannot edit circular pattern in a sketch

Anonymous — Fri, 24 Sep 2021 08:08:00 GMT

Tried to make a pattern using feature on the first body created with join, but no good, still gets N individual bodies.

Re: Cannot edit circular pattern in a sketch

g-andresen — Fri, 24 Sep 2021 08:26:23 GMT

Hi,

@Anonymous wrote:
Tried to make a pattern using feature on the first body created with join, but no good, still gets N individual bodies.

This is because you did not follow my recommendation and first extrude a base (without teeth) of the belt.

Watch the screencast and follow the timeline.

günther

Re: Cannot edit circular pattern in a sketch

Anonymous — Fri, 24 Sep 2021 08:24:31 GMT

I dont get what you write with "Extrude / Sweep the band with join". Tried to sweep with any possible combination of parameters, but didn't succeed.