Help with Polar array

[dammerel]

OS: Windows 8.1
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4572 (Git)
Branch: master
Hash: be2bb52796ae1be001882da114e8272c4c746af0
Python version: 2.7.8
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.7.1


With the attached model, how do i do a polar array of the hole around a PCD?
thanks andrew

[WalkingShadow]

Model is missing.

[dammerel]

Hi
i have uploaded the model
i want to put a series of holes around a PCD, the draft array is greyed out
any help would be appreciated

andrew

[jeno]

Hi dammerel,

if you want to use the polar array feature you need to have the hole as unique piece. You made a piece where the hole is part of the PCD.
In this case the wrong approach. It would be better to make first the PCD and than make the hole as separate pad. Then apply the polar pattern on the pad/hole.
I attached a model as visual aid

[dammerel]

Thanks Jeno
i was able to array as a feature - thanks
what if the center is NOT the 0,0,0 of the sketch?

andrew

[bejant]

what if the center is NOT the 0,0,0 of the sketch?

In the PolarPattern window, click on the default "Normal sketch axis", click on "Select Reference", and you can select an axis in the 3D window.

[jeno]

Thanks Jeno
i was able to array as a feature - thanks

your welcome. I think bejant already answered your question.

[dammerel]

again thanks guys
what sort of geometry can be used as the polar axis ? i tried a sketch point as the axis but that didnt work
i also tried the workfeature macro and put a workfeature point, that didnt work either

thanks andrew

[jeno]

Hello Andrew,
at the moment you are very limited. You can use an edge or the sketch origin. Mostly edges are not very useful exept you want to make an 90 degree array or similar stuff.
I am on 0.14.3702 which is not up to date. Maybe there are more possibilities in the new release.
The only thing that works for me is to use the sketch origin for the pocket and therefore also the polar pattern. But you can place the sketch for the pad (your PCD) relative to the sketch origin as you want. As english is not my first language I do not know how to phrase it better.
I attached a model as visual guide. Hope that helps.

[bejant]

i tried a sketch point as the axis but that didnt work
i also tried the workfeature macro and put a workfeature point, that didnt work either

Sorry, I wasn't clear enough. You can only select something that is geometry of your model, not something external like a separate Sketch or line. You can make a helper Pad and use an edge as the axis, but you'll have to:
Delete PolarPattern and Pocket,
Make a new Sketch002 on Pad,
Pad Sketch002 to make Pad001,

20150419a-dammerel.png (23.99 KiB) Viewed 3276 times

Detach Sketch001 and Reorient it onto Pad001,
Pocket Sketch001 to create Pocket,
PolarPattern Pocket by that "Select Reference", select an edge from the helper Pad001,
Make a Sketch on the helper pad on PolarPatter,
Pocket away the helper pad.

20150419b-dammerel.png (18.55 KiB) Viewed 3276 times

If you want to clean up the model and remove those residual lines you can use the OpenSCAD WB > Refine Shape tool.

Reading this again, it seems more complicated in print than it actually is by doing it.