topic Re: Bolt hole (or any hole) circle in Inventor Forum

Bolt hole (or any hole) circle

DustinBTW — Thu, 29 Apr 2021 20:05:37 GMT

Sigh, Why does such a simple command seem to be so difficult in this software? Seems like this would be a quick easy process in Solid Edge/solid works.

Sorry, I'm not hating on the software, I'm sure it's my misunderstanding of how to do it properly. Can someone please help.

I want to add centerlines to all these drilled holes in the cap, with center circles much like bolt center.

TIA.

Re: Bolt hole (or any hole) circle

swalton — Thu, 29 Apr 2021 21:03:13 GMT

Automated Centerlines Command?

https://help.autodesk.com/view/INVNTOR/2020/ENU/?guid=GUID-7EB10936-9A44-415C-9DDD-F0E50E209036

Manually add one?

https://help.autodesk.com/view/INVNTOR/2020/ENU/?guid=GUID-344E6E36-0BA6-4B13-89AE-A95ED91F94E2

Re: Bolt hole (or any hole) circle

DustinBTW — Mon, 03 May 2021 13:29:37 GMT

Neither of these features are working for me. Maybe it's because these are not patterns in the feature.

I am sorry, I thought the Video posted last time, I will post it now.

https://autode.sk/33cD8UV

Re: Bolt hole (or any hole) circle

johnsonshiue — Mon, 03 May 2021 20:29:32 GMT

Hi Dustin,

The took a quick look at the files. Indeed, these "holes" are not considered cylindrical holes qualified for automatic centerlines. The intersection edges are closed spline edges, not circular edges. You will need to create the center mark manually by selecting the closed spline edges individually.

Many thanks!

Re: Bolt hole (or any hole) circle

gcoombridge — Mon, 03 May 2021 20:12:42 GMT

Every second post on here seems to say I've had it - I'm going to change to solidworks, I think solid edge will be better... recently. They both have trial versions - try them out! The grass always seems greener..

After limited AutoCAD experience I learned parametric CAD on solid edge 20yrs ago and played with it again recently. (hated it!).

Re: Bolt hole (or any hole) circle

SharkDesign — Mon, 03 May 2021 20:25:00 GMT

Don't have Inventor on this laptop so I can't check your files.

Is this imported from step or another file type?

If so it won't work.

An option would be to use delete face > heal to get rid of the holes and draw them again properly using the hole command to allow Inventor to recognise them.

Not sure if cutting a hole across a curved face is your issue? As I said, I can't test it on this computer. If it is, my suggestion above probably wouldn't work either.

Re: Bolt hole (or any hole) circle

gcoombridge — Tue, 04 May 2021 02:42:57 GMT

Automated centreline does work for this. As @johnsonshiue said you can't select the geometry because the edges are not normal to the view. You can select the sketch geometry that created them however - share the sketch in the browser and then tick sketch geometry in the automatic center dialogue box. See attached screenshots...

Re: Bolt hole (or any hole) circle

DustinBTW — Tue, 04 May 2021 14:55:48 GMT

Thank you! This seems to be the best solution. Coming back to this today, I was thinking that maybe it was not working because the holes are not on a flat face. Using the sketch was an awesome solution!

I had found an alternative yesterday that involved creating a sketch onto of the view. This method seems better.