Creating a plane

[ToddPig]

Is there a trick to creating a plane that is tangent to a surface, and normal to an axis.

I have imported geometry, that has a hole through a curved surface.  In Solidworks, I would select the surface and axis, and it would create a plane that is normal to the axis and tangent to the curved curved surface (assuming it was not a spline).  This process couldn't be any simpler.  

In Inventor, the closest I can get is using the Normal to Axis through Point.  This gives a preview of what I want, but then gives the super helpful error message ...

Any help would be appreciated, thanks.

[mdavis22569]

Are you looking to do something like this? 

[ToddPig]

Mike,

Here is an image of the part I'm working with.  I would like to create a plane that is normal to the axis going thru the countersink hole and tangent to the outside curved surface.

[Curtis_W]

Hi ToddPig, 

Inventor does not have an option to create a tangent plane by selecting a curved face and an axis. Not sure why?

There is an option to create a tangent plane by selecting a curved surface and a point though. I've shown this option using a sketch point in this video.

What I'd typically do is create an work point on the loop of the hole by starting the Work Point tool and then right clicking and choosing Select Loop. 

The issue is this point is not created on the tangent of the surface, but just below the tangent, so it can't be used for creating a tangent work plane.

So what I do is create a work axis using just the columnar face of the hole, then create a work plane using the point and the axes.

Most often this suffices for what I need to do, but if not what I do then, is create the tangent plane by selecting the curved face and the new work plane. 

I tried to show all of that in this video.

Attached is an Inventor 2017 file for anyone who wants to experiment and might be able to show a better way.

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

[mdavis22569]

I still think it can be done ..sorry when I see surface, I was thinking surface type ..

However looking at it, it looks like it should be able to be done ..can you share the ipt or a section of it that has the holes?

[Curtis_W]

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@mdavis22569 wrote:

However looking at it, it looks like it should be able to be done 

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@mdavis22569

One assumption I'm making is that hole is not parallel/perpendicular to the origin planes, as in the part that I attached earlier.

If the hole in ToddPig's part is parallel/perpendicular to the origin planes, then you're right, this should be as easy as using the proper origin plane and the curved surface as selections.

@ToddPig if you can not attach the part file, can you confirm that the hole is parallel/perpendicular to the origin planes?

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

[ToddPig]

The hole is NOT parallel or perpendicular to the origin planes.  (If it was, then this would be a lot easier)

[mdavis22569]

? is there more than 1 hole? 

My thought is make a plane 90 to the Axis and then tangent to the hole ..

but that's just going from looking at it, vs working with it.

I don't think it would be a simple poof there it is, but I think it could be done ...

[Curtis_W · Accepted solution]

Hi ToddPig, 

After watching my first video again just now, it occurred to me that I was creating an extra plane.

See this new video for a better way.

Here I use the axis and  curved face to create a point (establishing location) and then I use that point and the curved face (to establish orientation):

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

[ToddPig]

That works.

* a few extra clicks than Solidworks, but good enough.

As always, THANKS!!!