Corner Cut Out

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MarcX
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Corner Cut Out

Post by MarcX »

Hi Friends,

I can't find an easy way in FreeCAD to cut out a corner on a part as you can see on the attached gif image.

Is there a simple way to do this ?
CutCorner.gif
CutCorner.gif (13.43 KiB) Viewed 2273 times
Have a nice day
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Marc BERLIOUX
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ppemawm
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Re: Corner Cut Out

Post by ppemawm »

MarcX wrote: Sat Dec 15, 2018 2:00 pm cut out a corner on a part...Is there a simple way to do this ?
Using PartDesign, if you know the coordinates of the vertices:
1. Attach datum points to each edge and then use attachment offset as required.
2. Attach the sketch to the three datum points

Picture2.jpg
Picture2.jpg (63.92 KiB) Viewed 2249 times
corner_pocket.FCStd
(18.43 KiB) Downloaded 52 times
You can do something similar if you know the cut plane angles by attaching a sketch to the corner vertex then
offsetting by the proper yaw,roll,and pitch angles.

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NormandC
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Re: Corner Cut Out

Post by NormandC »

Another method is to create a cube, rotate it and place it into position, then apply a Part Cut.

But this requires math. I try to avoid doing match as much as possible. ;)

Another PartDesign method, if the cut is even between the sides, is to simply create a sketch that is angled 45 degrees from the XZ/YZ planes, create a sketch with a triangle, and pocket it. It can be simpler to create a datum plane (PartDesign Plane) then attach the sketch to it.

In the attached FCStd file, I created a construction triangle (in blue) to control the width of the cut. In other words, it is the section that will be cut off, viewed from the top of the cube.
Attachments
corner_pocket_nc1.FCStd
(17.35 KiB) Downloaded 36 times
FC_corner_pocket_01.png
FC_corner_pocket_01.png (25.39 KiB) Viewed 2200 times
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MarcX
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Re: Corner Cut Out

Post by MarcX »

Hi,

Thanks to have moved my post in the right sub-forum and for the replies.

So I'm right, there is not a simple way to do this.. e.g. by selecting the three lines leading to the corner and then specify the length to cut.

As this is not a very different task than a chamfer it could be easy to add this feature.

Where is the right place to post a "Feature Request" ?

Bonne journée !
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Marc BERLIOUX
chrisb
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Re: Corner Cut Out

Post by chrisb »

Feature requests are discussed in "Open discussion".
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NormandC
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Re: Corner Cut Out

Post by NormandC »

Hello Marc,

MarcX wrote: Mon Dec 17, 2018 9:24 am So I'm right, there is not a simple way to do this.. e.g. by selecting the three lines leading to the corner and then specify the length to cut.
I've never heard of any CAD software that can do that, but I'm only familiar with mid-range CAD packages. I've never used high-end packages.

To me the usefulness of such a feature would be nil. But, to each his own. ;)
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Re: Corner Cut Out

Post by chrisb »

I found another way which I would not really recommend, because I don't understand completely what happens and how stable it is. I present it here hoping for some explanations.
  1. Create a PartDesign primitive cube 10x10x10
  2. Create a sketch. Map it to one of the standard planes, e.g. XY plane. It could be attached to its final position immediately but like this it is better to see what happens.
  3. Create a circle centered in the origin, radius 10.
  4. Open the attachment editor: click on MapMode, then on the ellipsis button.
  5. Click on the vertex where you want to remove material. The circle will lie flat on one side of the cube and have its center in the vertex.
  6. Click on "Reference2" and select the opposite vertex. You will get some warnings in report view.
  7. Remove the text from the second input field, it says e.g. "Box:Vertex6", the number may vary.
  8. Confirm, ignore the error messages and pocket to the depth of your desire. You may have to check "reversed".
  9. If you recompute the whole document no error is shown.
Now my question is, how can I see the difference between the state in point 5 and at the end of point 7. File is attached.
Attachments
CornerCut.FCStd
(10.19 KiB) Downloaded 39 times
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MarcX
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Re: Corner Cut Out

Post by MarcX »

Hi Folks,

Thanks ChrisB, I have tried your solution, but it's is only suitable for a cube:
6. Click on "Reference2" and select the opposite vertex..
If the shape is more complex or just 'rectangular', the datum plane is not going to be symetrically positioned around the first vertex.


I think (one day) I'll try to add some code to do this. I had a glance yesterday at the FeatureChamfer source files to find out how to get the selected edges. Maybe through the Base.getSubValues() method.

Anyway, the question was about a simple way to do this and it's not that simple..

Sorry for the noise

Et Bonne journée !
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Marc BERLIOUX
triplus
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Re: Corner Cut Out

Post by triplus »

Corner.png
Corner.png (47.69 KiB) Viewed 2040 times
Another way:

First sketch provides the corner edge length parameter. Second sketch provides the third reference point. Third sketch is attached by using the three points as a sketch plane and geometry reference, and is extruded after. Cut between Box and Extrude feature produces the Corner.
chrisb
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Re: Corner Cut Out

Post by chrisb »

MarcX wrote: Thu Dec 20, 2018 11:29 am Thanks ChrisB, I have tried your solution, but it's is only suitable for a cube:
I have hijacked your topic because this solution lied on the way. However, I would not recommend it anyway, before understanding how to control it.
NormandC wrote: ping
Normand, do you have an idea how to distinguish the attachment from my step 5 above from the attachment after step 7?
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