I have a box model and i wish to remove just one corner . The flat plane so created would intersect on three sides and 3 adjoining edges. A chamfer if you like but across one corner point and not along a single edge.
Does anyone have any idea how this could be achieved ?
Solved! Go to Solution.
Solved by karyeka. Go to Solution.
Solved by carl_bass. Go to Solution.
Here's one way but there are certainly others
Sketch a line on the top face
Then construct > plane at angle at 45 degrees from that line
Then go to Modify > Split Body and there should be a second body created
Either turn off the visibility on the second body or delete it
A drop more complicated than seems necessary but it's a fairly general way to do it
Hey LJHFUSCAD,
I think I found a quick way to accomplish what you're trying to do. Here are the steps I took:
1. With my Box modeled, I first create a construction plane that passes through 3 corners by using the Plane Through Three Points command found under the Construct Menu.
2. Select Three corners to create your first construction plane.
3. If this is the corner of the Box you're trying to remove, then you can skip to the last step! If not, we now need to offset a construction plane from the one we just created (it will be parallel). To do this, we'll use the Offset Plane command found under the Construct Menu.
4. Create an Offset Plane from the previously construction plane, and move this plane to the area you like.
5. The final step is to remove the corner of the Box using the Split Body tool found under the Modify menu. In the Split Body command, set the Box as your Body to Split, and select the appropriate construction plane as the Splitting Tool. You'll see that you now have two solid bodies in the browser, and you can delete/hide the unwanted corner.
Let me know if this helps!
Taylor
And here's a slightly different way. Just make a box as a new body on top of the existing box
Then use the move commsnd to orient it to the right place
And then use modify > combine using the cut option to get rid of the corner
So there's 3 different ways and I'm sure there are more
Another way is to chamfer the 3 edges that come to the corner. Then select the 3 chamfered faces but not the vertex cap and delete them. This delete is delete with heal where the adjoining faces are extended to heal.
Please check the video - https://screencast.autodesk.com/main/details/fd72d356-0868-4e37-8132-755e00221f8a
Thanks,
Anand
Fusion360 Development
In order to add the corner chamfer Fusion 360 would need the ability to apply a chamfer to a vertex. I believe this a good suggestion and I recommend you create a post in our IdeaStation to gather support around it. We use the IdeaStation for customer feedback as well as a way for our community to influence priorities to our development backlog.
Link to IdeaStation
https://forums.autodesk.com/t5/forums/postpage/board-id/125
Cheers,
Mike Prom