Hole Table Origin Selection

[karthur1]

I need to create a hole table for a part.  I would like the origin to be at the center of the part.  Problem is there is not a round hole at that location.  Attached is a similart part.  The one that I am doing is much larger and has many more holes... this is just an example.

How can I pick this as the origin of my hole table?

Thanks,

Kirk A.

Windows 7 x64 -12 GB Ram
Intel i7-930 @ 3.60ghz
nVidia GTS 250 -1GB (Driver 301.42)
INV Pro R2013, SP1.1 (update1)
Vault Basic 2013

[GSE_Dan_A]

Could you create work planes and then use the Split tool to split the face of the part so that the face forms 4 quadrants.  There by being able to place your Origin at the intersection? 

Only catch is that you will have to change the properties of the split lines in your drawing to white in order for them to not show up when printing.  I am sure there is an easier way to do this....

[Curtis_Waguespack · Accepted solution]

Hi karthur1,

In additon to the previous solution you can use a workpoint to do this.

In the part file click the Point button

Then right-click and choose Loop Select,

Then choose an outer edge of your rectangular face to create the work point at the center of the loop.

In the drawing, create the view,

Then expand the browser node for that view and locate the model tree,

Right-click on the workpoint node and choose Include,

Then use the included workpoint to place the origin.

You can then right-click on the workpoint in the browser and turn off the visibility.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[karthur1]

Thanks Curtis... using the workpoint works great.  I was not able to use the split command cause there was not an edge there.  There is an opening where the two planes intersect.

[isabel.gruenhagen]

Along these lines, is it possible to select axes instead of a point?  For instance I want to place my origin at the corner of a part--yet I had to chamfer the corner (so the ideal point to select is now gone).  Solidworks allows one to select axes instead of a single point.  Does Inventor offer the same capability?

[Curtis_Waguespack]

HI isabel.gruenhagen,

Welcome to the fourm.

You can do the same thing with an axis.

• Use the End Of Part (EOP) marker to "rewind" the part to before the chamfer was applied
• Then create the work axis
• Then move the EOP back down to the end of the part

• In the drawing, create the view

• Then expand the browser node for that view and locate the model tree

• Right-click on the work axis node and choose Include , it will come in as a 2D point

• Then use the included work axis (the 2D point) to place the origin.

• You can then right-click on the work axis in the browser and turn off the visibility.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[isabel.gruenhagen]

Thanks for answering!  That sounds awfully in-depth though... curious why Inventor can't do it in one single step like SW.

[Curtis_Waguespack]

Hi isabel.gruenhagen,

Maybe you're just looking to move he origin as described here:

http://forums.autodesk.com/t5/inventor-general-discussion/ordinate-dimension-datum-location/m-p/6055...

Or use the yellow "tracking" dots to find the corner:

http://forums.autodesk.com/t5/inventor-general-discussion/ordinate-dimension-datum-location/m-p/6055...

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[isabel.gruenhagen]

Somewhat delayed, I know... it seems that both those links take me to the same page and I am curious what the second one was supposed to be.  I do not care to move my origin, though perhaps tracking dots would resolve my issue.  Have you created a table in Solidworks using the method I described?  It's incredibly straightforward.

Thanks!

[Curtis_Waguespack]

Hi isabel.gruenhagen,

The second link should have gone to something like what is shown in this video.  It's been a while since I've created a hole chart in Solidworks.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com