Hi all,
In the attached part, I am trying to show a hole drilled at a compound angle. I have attached a pic of what the part is supposed to look like. I am having trouble laying out the plane on a compound angle. The hole should be centered on the width of the flat and drilled through. 15° angle one way and 20° another way.
The ipt file attached is really messy in attemps to acheive the compound angle. Please feel free to offer any suggestions as to what I am doing wrong. I can't seem to wrap my brain around this.
I am using Autodesk Inventor 2013.
Thanks
Mike
Solved! Go to Solution.
Solved by CCarreiras. Go to Solution.
This may or may not be the BEST way to do it ... but this is a way to do it.
Ignore the errors in the file about the missing iLogic rule, if you get any.
I use Sketch 2 and Sketch 3 to lay out the two angles that I need, from a common starting point.
3D Sketch 1 has an intersection curve bringing Sketch 2 and Sketch 3 together to give me the axis of the hole, which then gets a work axis dropped on top of it.
Because the hole will not be drilled normal to a plane, I set a work point on the upper face of the cylinder, then a hole feature using the ON POINT option. Use Work Axis 1 to define the direction of the hole - you may need to flip direction.
Because you're not starting normal to a face, you'll have a little bit of material left at the top of the hole. Delete face + heal will take care of that.
Use a circular pattern, then you're done.
Edit: Ah crap - just realized you've got 2012. My file attached here is 2013. 😞
Rusty
Hi!!
All you have to do is create a axis with de correct direction.
For achieve this axis (A) you have to do some work features.
1- Begin by create two axis:
Create axis 1 selecting the sketch point (you already have this point) and the plane xz.
Create axis 2 selecting the sketch point (you already have this point) and the plane xy.
2 - Now you will create two angle planes:
Create plane 1 selecting the axis1 and the plane xy, give the 20 degrees (or 110, or another equivalent, depends the direction you chose).
Create plane 2 selecting the axis2 and the plane xz, give the 15 degrees (or 105, or another equivalent, depends the direction you chose).
3 - Now create the final axis you need:
Create axis selecting the plane 1 and plane 2.
4 - Create a construction point:
Select the sketch point to create this point.
You can see all the construction elements in the browser in the image below.
5 - To create the Hole.
Select the tool “Hole” and select hole by POINT.
Now select the construction point and the AXIS A. Chose correct direction and deep.
6 – you have to adjust the hole.
Use delete face with the option Heal and chose the face in the image below, click OK and that’s it!!
Sorry, I don’t have INV 2012 installed so I can’t send you the model, but I hope you can do this with this explanation.
Regards
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Many thanks for your concise explanation. Very detailed. This helped me very tremendously.
Mike
Hi!
I use a lot this "Hole by a Point", the question is that little portion of material that remais above...
Was a good improvement if Autodesk solve that question in next versions... Autodesk Techs... take a look on that...
Glad to help, bye.