Sketch edition produces a mess on other sketches

[bitacovir]

I have the problem when I want to edit a sketch in a geometry (deleting lines) because this changes other sketches.

sketch_1.gif (894.54 KiB) Viewed 1258 times

kitchen_furniture5.FCStd

(301.09 KiB) Downloaded 31 times

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.12223 (Git)
Build type: Release
Branch: master
Hash: 917e61a3be12f3316d571ebf6fd6e3c537691c14
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0
Locale: English/Australia (en_AU)

[microelly2]

When you delete or add geometry in a sketch the numbering of faces and edges in depending objects changes.
So sketches which are connected to a face are moved to other faces.
this is related to the topological naming problem.
So the tipp is: do not change the topology of a sketch which has depending sketches.

[bitacovir]

Ok. I think I can extract DXF drawings to make the edition with libreCAD.

[NormandC]

I think I can extract DXF drawings to make the edition with libreCAD.

That's hardly a good solution, since you need to use a separate software.

Without changing how you made your model, what you can do rather than editing TeethProfile and removing one of the rectangles is to simply add a new sketch and Pocket to remove the unwanted tooth. But that's just a workaround.

What would be more appropriate is to not map your sketches to faces when you have another choice (i.e., standard planes). I mentioned it in the FC v0.17dev: Part Design Next Usecases and Best practices topic.

I understand that your "Tooth" and "TeethProfile" sketches need to be mapped to the faces of the solid. But "LatHole" and "Sketch006" could have been attached to the YZ_Plane and XZ_Plane, respectively. Doing so, they would not be affected by topological naming changes. This would make your model moderately more robust.

To get a much more robust model, you would need to use skeleton geometry, that is create datum planes that would define the outer dimensions of your model; for example, create a datum plane offset from XZ_Plane that would define the back wall of the part. When creating the Base sketch, you would use external geometry linked to the datum plane; then, rather than attach the "Tooth" sketch to the back wall of the solid, you would attach it to the datum plane.

On the other hand, it's not too much difficult to repair a model with not too many features by remapping the sketches to appropriate faces using the https://www.freecadweb.org/wiki/images/ ... Sketch.png Sketcher MapSketch tool.

So, you have quite a few alternatives that do not require using a third-party CAD program to edit your model.

P.S. Have you played with the "Set tip" command? Your Walls001 tip is set to "LatPocket", which is not the last feature in the tree. Moreover, the Mirrored feature should actually be the last one in the tree, but "RearPocket001" is below it - which is odd, because Mirrored uses it... (I think I have seen the same issue on the forum in the last week or so)

How to fix your model:

1. Activate the body Walls001
2. Right-click on Mirrored and select "Set tip"
3. Right-click on RearPocket001 and select "Move object after other object"
4. In the dialog that opens, click on the drop down menu and select "LatPocket" then click OK.

[bitacovir]

I think I can extract DXF drawings to make the edition with libreCAD.

That's hardly a good solution, since you need to use a separate software.

Without changing how you made your model, what you can do rather than editing TeethProfile and removing one of the rectangles is to simply add a new sketch and Pocket to remove the unwanted tooth. But that's just a workaround.

What would be more appropriate is to not map your sketches to faces when you have another choice (i.e., standard planes). I mentioned it in the FC v0.17dev: Part Design Next Usecases and Best practices topic.

I understand that your "Tooth" and "TeethProfile" sketches need to be mapped to the faces of the solid. But "LatHole" and "Sketch006" could have been attached to the YZ_Plane and XZ_Plane, respectively. Doing so, they would not be affected by topological naming changes. This would make your model moderately more robust.

To get a much more robust model, you would need to use skeleton geometry, that is create datum planes that would define the outer dimensions of your model; for example, create a datum plane offset from XZ_Plane that would define the back wall of the part. When creating the Base sketch, you would use external geometry linked to the datum plane; then, rather than attach the "Tooth" sketch to the back wall of the solid, you would attach it to the datum plane.

On the other hand, it's not too much difficult to repair a model with not too many features by remapping the sketches to appropriate faces using the https://www.freecadweb.org/wiki/images/ ... Sketch.png Sketcher MapSketch tool.

So, you have quite a few alternatives that do not require using a third-party CAD program to edit your model.

P.S. Have you played with the "Set tip" command? Your Walls001 tip is set to "LatPocket", which is not the last feature in the tree. Moreover, the Mirrored feature should actually be the last one in the tree, but "RearPocket001" is below it - which is odd, because Mirrored uses it... (I think I have seen the same issue on the forum in the last week or so)

How to fix your model:

1. Activate the body Walls001
2. Right-click on Mirrored and select "Set tip"
3. Right-click on RearPocket001 and select "Move object after other object"
4. In the dialog that opens, click on the drop down menu and select "LatPocket" then click OK.

Dear NormandC. Sorry, I had not seen your response before.
Thanks to much for your deep analysis of my project and your observations. I will follow your indications carefully. This is my first time working with FreeCAD and sketch tool. I hope to publish images of the built product, soon.
Thanks again for your time.