Is there a way to add center reference axes to the (8) holes in the attached part?
I would like to made screws to the holes.
I tried playing around with various workarounds with no luck.
Thanks for any help.
You can add reference points to the center of the face for the holes. Then draw 3d sketch lines with the endpoint of the line coincident with points. Then make those lines perpendicular to the surface.. Really not that much work when you get the process down.
If you do indeed want axis (rather than sketch lines.. You can do a surface sweep and get the axis. Although that is probably not necessary. I did that on one hole to show.
Future Version! Could you post an image please?
Here you go Rob.
Thanks for posting the pic, Glen.
Since the holes are no longer perfect cylinders your life is a little more difficult. You might be best off to use a 3D sketch and draw a circle and pick three points on the edge of the hole spaced as far apart as possible to constrain the circle. With a planar circle you can then construct a normal axis. It will be some work to do this.
What about the mating parts? Wouldn't the holes on them be true cylinders? That would be a better reference for mating your fasteners.
There are no holes in the mating part.
Sheet metal screws will be mated to the part I attached.
Okay. . . So you will make holes on the mating part by virtue of running the sheet metal screws in? If that is the case then the precision for the screw mates in these holes isn't so tight. Go to my earlier suggestion about making a 3D sketch, but mate the drawn circles to three convenient points on the edge of the hole. You are trying to find a reasonable center and a reasonable normal.
I would be inclined to mate this up like Dennis Dohogne suggests. That would be more true to reality as this part wouldn't be controlling the location. To keep this part from rotating, you could then just make a hole edge tangent to the fastener.
Tried it on my part (using yours as a reference),it worked! Thanks!
Can you create reference Geometry in the Assembly?
Michael, I think I found a way that works pretty decently.
Insert -> Reference Geometry -> Point
Then select the inside surface of a hole and the default it should choose is "Center of Face". If it doesn't do that automatically, choose that.
Then select the option "Projection". For your "Selections", choose the "Point" you just made, and then the front face of the ring.
Insert -> Reference Geometry -> Axis
Then create an axis between your two constructed points.
Give it a try and let me know how it works.
I like it, but could I suggest an alternative? Eliminate the axis. Place the screw with two concentric mates, one to each point, and a third mate coincident from the bottom face of the screw head to the second point (the one on the surface), to fully define its position. The screw in the screenshot below is only able to spin (for some reason Lock Concentric Rotation isn't available when a Reference Point is involved, at least not for me).
Then it would be pretty easy to place the rest of the screws using the "Copy with Mates" function (pinned until they're all inserted).
This would also work, good stuff. Thanks!
I have had good luck selecting the inside face of the hole.
Some great ideas here
Im on 2015 so have recreated something similar. I used a preliminary wrap feature to scribe some 'pie slices' that gave a vertex to define an axis before they are cut away
Some really helpful replies to this one. I learned a lot here. Thanks guys.
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