Hole placement on a Cylindrical object

[Lonnie.Cady]

I have a cylindrical part that needs to have a set of holes placed radially.  I have the hole on the radial face and can see how to adjust the center angle with the manipulator or the dialog box.  Can someone explain how to positoin the hole axially?  I assumed that I would select an edge and ad a dimension, but have not been .

[innovatenate]

Since the circular face will only enable you snap to the center point in the hole command, you may consider creating a sketch with a point located in the desired position for the centerpoint of the hole. Does this help? Please let me know if you have any other questions.

[Lonnie.Cady]

I will try this later, just don't remember being able to lock the hole to a sketch point.  If sketch changes is the hole going to move with it?

[innovatenate]

The trick is to select the sketch point when placing the hole. If you update the sketch, the hole should move to the new position of the sketch point. I hope that helps. Let me know if you have any other questions. 

Thanks,

[Lonnie.Cady]

Thank you, I will test when I get home.  Are you considering this a work around or the desired behavior.  This seems to be a little more complicated than it should be.  Not being critical but I have several radial holes in my parts and creating a skectch just to place a hole seems like it could be improved on.

[innovatenate · Accepted solution]

I would say the hole command is working as designed in this case. With that said, there is always room for improvement and your feedback is very much appreciated. The IdeaStation is the best mechanism to suggest feature enhancements or improvements. This will let the product management team know what you want to see implemented in future releases.

http://forums.autodesk.com/t5/ideas/v2/ideaexchangepage/blog-id/125

If you post a link back to this forum thread. I will vote it up!  Let me know if you have any other questions.

Thanks,

[sanderk]

Can somebody explain how to do this the right way? I just can't get it to work properly.

I can't sketch directly on the cilinder wall, right? But if I make a tangent construction plane then I can't specify what the angle is compared to the cilinder and it doesn't snap to any point, it just seems to be oriented to the first point that I pick, which is basically random.

If I draw a line from the cilinder origin to the point where I want the hole then I can select the right point to make a hole but the hole will be at a 90 degree angle. So that doesn't work.

Then I make an offset plane at the distance that I know the cilinder is wide. I draw a line with one point where I want the hole to be. I make a hole and select the point and there is my hole in the right location. But now the hole is not on the cilinder. If I move the hole it will not move on the cilinder but on a plane in front of the cilinder and I can't specify a center angle. So now my solution is to to create a hole in the middle where it will snap to my sketch line and then create a circular pattern where I can select an angle. But this seems rather complicated, no?

[innovatenate]

If you edit the tangental construction plane (assuming timeline is on), there should be an option for Angle in the Edit dialog. Can you use this angle to get what you need?

I hope that helps. Let me know if you have any questions.

Thanks,

[schneik-adsk · Accepted solution]

To position axial. Place the hole. Select the manipulator for the hole position. You should be able to drag it and see the hole slide up and down the shaft. Stop draging, and move the mouse ofer the end face. It will highlight. Click and you will get a dimension from the cap face to the hole point. You can ow enter the precise distance of the hole from the end cap face. 

Was this what you were looking for?

[sanderk]

Thank you for your answer.

Yes, I see an angle. But as far as I know the angle is relative to the first point you clicked on the cilinder wall and since it doesn't snap to anything (I tried), that point is not a precise reference. I could be close to something or even be exactly but there is no way of knowing since there is no reference in the dialogue. Or am I missing something?

[sanderk]

Ahh! You're right! It does give a distance if you click the manipulator and then the cap!

From the answers above I was assuming that it didn't and somehow I didn't get it to work either. I guess it's a matter of following the steps in the right order.

Thanks!

[Lonnie.Cady]

@schneik-adsk @innovatenate

When placing radial holes I can select the radial face and dimension from the end of the part or cap as mentioned in previous post.  What is the reference plane for the angle manipulator?

Also I noticed that when I open back up to edit the center angle changes back to zero.

Thank You.

[LibertyMachine]

@Lonnie.Cady it appears that any plane CAN be used to define an angle off of. It seems to default to the X plane, but that may be dependent on how it's drawn. If you have your Origin turned on, you can select one of the faces and then specify an angle. This can also be used by creating a "Plane at Angle"

I too am seeing the value reset back to zero. Mind you, the hole location stays the same, it just reverts it's angular dimension back to zero @innovatenate is this expected behavior, or grounds for a ticket?

[Lonnie.Cady]

@LibertyMachine thanks.  I was struggling to see how to reference the plane at first.  Once I clicked on the angle manipulator I was able to select a plane for reference.  I get a little concerned with the ability to set a dimension and then arbitrarily drag the hole again.  Makes me a little nervous like things are not locked down.

Also once I open a hole up to check it or modify it with out the reference plane and angle I set being displayed I am kind of forced to start over.

[LibertyMachine]

No, it certainly has room for improvement. At least highlight the selected plane and show the angle with leader lines. Surely this must be a feature not yet fully developed...?

[Lonnie.Cady]

@LibertyMachine something also seem strange.  Once you snap to a plane and set an angle to say 20 deg and close the hole command, when you modify that hole not only is the center angle set back to zero but when you try to snap back to a plane it sets the center angle to 70 instead of 90 so everything seems to have rotated.  

Not sure how to explain but you can't really snap back to a 0deg or 90deg reference once you set an angle and close the hole tool.

[Lonnie.Cady]

@LibertyMachine I think for me the most sound method will be to create a tangent plane at the proper angle create a hole on that plane at this point.  

[LibertyMachine]

I saw the same thing. It's like it adopts the orientation of the selected plane and sets it (the rotation angle) to zero and the physical orientation normal to that plane upon closing the dialog. So, you would need to calculate backwards.

[Lonnie.Cady]

@LibertyMachine

Well that tangent plane seems to have almost the exact same problem.  I guess I will have to create an extra sketch and then use tangent at point.