Sketcher clone

[lah]

Hello,

I'm trying to use sketcher clone. In file attached

clone_sketch.FCStd

(50.21 KiB) Downloaded 27 times

when I clone the sketch, the constraints on clone sketch is not linked to source sketch.
Is it normal ? How can I solve this issue?

clone_issue.PNG (46.25 KiB) Viewed 1250 times

My goal would be to have such thing : an array of this extruded part

clone_issue_extrusion.PNG (16.12 KiB) Viewed 1250 times

But because clone seems to have an issue, now I have following alternatives to achieve it :
* extrude sketch (without the clone) and use part design clone. To be used with some constraints in a spreadsheet to be used to position cloned bodies. The drawback with this solution is that now I'm getting lot of new bodies
* Use array tool of draft workbench on a body that needs to be repeated. Straightforward.
What are best practices?

OS: Windows 10 (10.0)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.22846 (Git)
Build type: Release
Branch: master
Hash: 1f46b72491a0008384a6db4f2615a656249f6f08
Python version: 3.8.6
Qt version: 5.12.5
Coin version: 4.0.0
OCC version: 7.4.0
Locale: French/France (fr_FR)

[chrisb]

Use PartDesing->LinearPattern. it stays all in the same body.

[lah]

I tried it first that's why I came across this issue, why?

I needed to do a 4x4 x-axis/y-axis repetition of this pad. Linear repetition helped me to do a x-axis OR y-axis repetition.
So I did x4 x-axis repetition on x and tried to do a a 4x linear repetition on y-axis with from this first linear repetition. It's not possible to a linear repetition from a linear repetition

So I thought another solution would be to use sketcher clone tool to have 4x the sketch on x-axis and apply a y-axis linear repetition on resulting pad. At this time I faced this clone issue...

[user1234]

You made no clone sketch, you made 4 rounded squares in one sketch.

[lah]

Maybe it's not clear above, what I'm trying to use is Sketcher clone tool on 1 rounded square to have 4 similar rounded square in same sketch.

[user1234]

The sketcher clone tool works only on proper constrained elements. For you the way to go make a pattern like chrisb said.

Greetings

[jmaustpc]

Guy's he is talking about using the Sketcher functions, Copy/Clone/move and Array on a set of sketcher geometries within a sketch in edit mode.

I just quickly tested his file in both 0.19 from the stable and daily PPAs. It is only working in "Copy" mode with both copy and clone, and Array is also only working in "Copy" mode when you select "clone" mode.

FreeCAD is not producing the "equals" constraint etc in the "clone" option, it is just doing what "Copy" is expected to do, because of the way the OP has applied their constraints. The constraints are all applied to between two different geometries. So for example his top line length is determined indirectly by a constraint that gives the horizontal distance between the two end points of the two vertical lines.

pinged by pinger macro

Perhaps Abdullah might be interested in this? I suspect he will say it is not a bug, it is a feature limitation hence a feature request, not a bug report.

I just tested in my own new file in FreeCAD 0.19 from the stable PPA and Sketcher geometry Copy/Clone both worked as the OP expected with a fully constrained sketch where those constraints are applied to a specific geometry. Here is the example file...

copy_clone_tests_sketcher_fully_constrained1.FCStd

(10.68 KiB) Downloaded 26 times

And a screen shot

Screenshot_20210419_223618.png (127.84 KiB) Viewed 1155 times

In this next file I demonstrated both direct and indirect constraining of a rectangle by first in the top left quadrant I constrained the edges of a "rectangle". Where as the bottom right has it's sides determined bu H and V distance constraints of the different lines. The different lines on the lower left are the same as the bottom right but without the coincident constraints on the end points. Here is that file...

copy_clone_tests_sketcher_constrained_only_between_geometry2.FCStd

(9.61 KiB) Downloaded 24 times

and a screen shot of that

Screenshot_20210419_223646.png (74.69 KiB) Viewed 1155 times

So in summary FreeCAD is working as expected if the constraints are applied directly to a geometry, it's just about how the constraints were applied, they were not applied directly to the geometry item so FreeCAD copied in "copy" mode rather than "Clone" mode.

The OP could apply the expressions manually, either directly with in the sketch or via values held elsewhere e.g. in a spreadsheet.

Regards
Jim

OS: Ubuntu 20.04.2 LTS (KDE/plasma)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19. both daily PPA and Stable PPA
Build type: Release
Branch: unknown
Hash: e8566f22bbeb0b7204e3c45519d0963e8881100b
Python version: 3.8.5
Qt version: 5.12.8
Coin version: 4.0.0
OCC version: 7.5.1
Locale: English/Australia (en_AU)

[Bance]

Maybe Use multi-transform?

[lah]

@jmaustpc thanks for the precise answer.

So in summary FreeCAD is working as expected if the constraints are applied directly to a geometry, it's just about how the constraints were applied, they were not applied directly to the geometry item so FreeCAD copied in "copy" mode rather than "Clone" mode.

The OP could apply the expressions manually, either directly with in the sketch or via values held elsewhere e.g. in a spreadsheet.

[abdullah]

Perhaps Abdullah might be interested in this? I suspect he will say it is not a bug, it is a feature limitation hence a feature request, not a bug report.

If I remember correctly, back in the day there was no expression support yet. This means that the only substitution possible for clone is for a dimensional constraint applied on a single geometry element. Today I guess the tool could be extended to link the remaining dimensions via expressions. Feel free to file a ticket for a feature request.