blind hole at angle

stuart_hatherway · September 2018

Hi

I'm trying to insert a blind hole at an angle. I read up and it was suggested drawing a 3D spline along the path the hole will follow and then setting a point normal plane off of the vertex to work from .

https://cad.onshape.com/documents/daa688d1b3b989d5fdf5001c/w/ea7c5d76f41bf1a12544120b/e/2640139bf2e3c200e4f58546

I have done this but cant seem to locate the hole at the end of the spline and face of the plane.

Any ideas would be appreciated or is there an easier way to do this. Thanks

regards Stuart

philip_thomas · September 2018

This should get you going in the right direction

https://cad.onshape.com/documents/5d3462b436a8cf4265e728a6/w/fcd6c0280c91a52556d70e4a/e/d2b097057ddd9462df292013

TimRice · September 2018

In order to use the Hole feature to create a hole through the part you will need a point and a plane perpendicular to the hole axis. You got the plane component but you will have to create a sketch on the plane and add a "point" where the spline connects with the plane. Please see my version here:

https://cad.onshape.com/documents/a3e1c5175b3501dc1d54221b/w/d638e5ad4b47b3b9629ab0e3/e/accaffa1550d2d9e7ce4bfe0

Jake_Rosenfeld · September 2018

Hi @stuart_hatherway

Looks like you're almost there! Only sketch points can be used to make holes, so in sketch 6 you'll have to "use" the endpoint of the 3d spline:
https://cad.onshape.com/help/Content/sketch-tools-use.htm

Then once you have the point in the sketch, you can use it as a selection for your hole.

Once I did this, I was able to make the hole, but the geometry was weird because the starting plane of the hole cut through the model:

My solution for this was to make the plane exist entirely outside the model by using a line-angle plane off of the top edge of the part (using the 3d fit spline as a reference for the 'angle' parameter):

And then when the hole is built, it looks correct!