CAD Forum

So, I have a cylindrical face and an existing 2D sketch defining points coincident with that cylindrical face.

When I use the hole wizard and go to place my holes, it is not working. I figure its an order of operations or a small technical issues but I haven't been able to sort it out yet.

Here's what I'm doing:
1.Start Hole Wizard
2. Configure Hole
3. Select the appropriate body (Multi-Body Part)
3. Change to Positions
4. Select Cylindrical Face
5. Try to selct sketch points = FAILURE

Thoughts?

Error Message: Points to locate holes are not valid. They may not be constrained or may be located on edges or vertices

For some reason, it doesn't want to let you make your hole locations coincident from within the hole wizard. You can, however, just put some hole locations on the surface, then exit the hole wizard, and then go back into the 3d sketch and make the points coincident.

Beuatiful, Thanks!

I did a little playing around, and got the same error message in some situations. However, I was able to get it to work in either of two situations:

1. If I I selected a 2d sketch for the Hole Wizard points, in which case it would of course put the holes perpendicular to the plane. . .

2. . . . or when the existing sketch points were on (coincident with) the cylindrical face.

If you think about it it makes sense. If the point you're referencing isn't on the cylindrical surface, and you've selected the 3d sketch option in the Hole Wizard, then the software doesn't know how the hole should be oriented. It knows you want the axis coincident with the sketch point, but it doesn't know the orientation (or direction) of the axis

If the Hole Wizard sketch is on a 2d plane or face then it knows the axis is perpendicular to it. If it's on the face of the cylinder it knows the axis is perpendicular to an imaginary plane that's coincident with the point and tangent to the face.

Make sense?

Edit: The above is what happens when I over explain.

LOL! We are birds of a feather when it comes to explanations.

So about #2...

My points are coincident with the cylindrical face (at least they were, I redid the sketch as a 2D just to try something different). I received the same error. I mean, techically they are STILL coincident with the face mathematically if not relationally. And, as I said, I made a separate 3D sketch as my first attempt. So, they were for sure coincident with the cylindrical face unless SW automagically changed something at some point.

This is really buggy behavior. If you just drop a point anywhere to prevent the error message and then go back and attempt to edit the 3D sketch and try to add new points coincident to where you originally wanted them, you get no error message but you also get no holes. The points are there, but no holes are created for them. If you then delete the first point you placed, the error message comes back.