[Solved] Polar pattern where certain instances are left out

[Alexanderw22]

Hello everyone,

I am quite new to FreeCAD and I have been stuck on the following problem for a couple days now.
I would like to use a polar pattern of ridges in which certain ridge instances are left out. In the place where 3 instances are left out create a bigger pocket with a larger diameter. To better illustrate my questions see the pictures below. I would like to achieve a combination of the two.
Problem is that in the first file I use the Draft -> Array tool to create a polar array of 48 of the body created in Part design. Then I use the Part -> Compound Filter to filter out specific items using index numbers of the array. Then I use Part -> boolean fragments (which takes a long time to calculate ~10min) and then another Compound Filter on top of this. The problem is that all these operations are created outside the body which limits the ability to edit the body (to add the 6 bigger pockets). Also the Part -> boolean fragments part is very inefficient.
In the second file everything is done in the Part Design section with two polar patterns for the larger and smaller ridges. This operation is far more elegant however I was unable to limited the instances of the polar pattern in part design

Screenshot 2019-11-05 at 17.18.54.png (267.6 KiB) Viewed 1197 times

Screenshot 2019-11-05 at 17.18.02.png (375.43 KiB) Viewed 1197 times

[Vincent B]

Share your file then we will get a glance.

[chrisb]

From what I have read here, Lattice workbench could be of help with this task.

[kisolre]

Try multitransform with two pollar patterns - first the oner near each other then 5 at 360 deg.

[Alexanderw22]

I have read about the lattice toolset on another post. Up to now I was not yet able to understand how that toolset works.

Here is a link to both files mentioned in my first post:
(They were too large to upload to the forum directly)

Thanks for taking a look!

[DeepSOIC]

Up to now I was not yet able to understand how that toolset works.

That's not unexpected, you are not alone.

A quick how-to:
0. make sure the body is activated.
1. create a polar array of placements (paperplanes) with all (unfiltered) occurrences
2. filter unnecessary occurrences with ArrayFilter tool (it is like CompoundFilter, but for arrays of placements)
3. apply Lattice PartDesign pattern to the features you use to cut one ridge
done.

alternative:
0. make sure the body is activated.
1. create a polar array of placements (paperplanes) one set of ridges (edit SpanEnd property, you can also quickly make such an array by making a sketch with an arc first, and creating the array when the arc is preselected)
2. create another polar array with however many groups of ridges you need
3. combine the arrays using "Populate with copies: build array" tool
3. apply Lattice PartDesign pattern to the features you use to cut one ridge
done

[DeepSOIC]

Here's an example file for the "alternative" approach

[freedman]

Typically in an additive workflow you would fill in the slots you don't want and then do something different. Using a copy of the original sketch you can pad/fill the groves with the original shape. You can do singles by placing a datum plane at angle or do many in an array fill.

[Alexanderw22]

This rundown, (quote below) together with the attached file with the second method did the trick for me. Seeing a lattice pattern that works and being able to edit it and see what effects it has on the output helped me a lot!

A quick how-to:
0. make sure the body is activated.
1. create a polar array of placements (paperplanes) with all (unfiltered) occurrences
2. filter unnecessary occurrences with ArrayFilter tool (it is like CompoundFilter, but for arrays of placements)
3. apply Lattice PartDesign pattern to the features you use to cut one ridge
done.

Thanks guys!

[Vincent B]

hi,
I've got an error with LatticePattern. The Y positions seems not working.
Where my mistake? An other question: why not use a Binder to use it as a lattice?
thx