Cannot Create a Midplane Work Plane in a Weldment

[petestrycharske]

All,

I have been working with an assembly that is based on Multi-solid body part model and my particular location is away from the origin.  I have come across a situation where I need to create a midplane on one of the parts in the assembly to help mirror some other components.  One of the great enhancements in Inventor 2015 is the ability to create a midplane between two angled planes, but I cannot seem to get it to work in my weldment assembly.  I ran across a post (here) that seemed to indicate that created assembly level work features could be problematic or at least must be applied differently than in a part file. 

My situation is that I want to create a midplane between two angled planes using just one of the parts.  I am able to select the first plane, but not the second plane on the same part.  However, I can select the second plane on a different part.  Is there some kind of limitation that won't allow me to choose two planes from the same part in the assembly?  I have attached a couple of screen shots to help illustrate what I am talking about.

I can work around this, but thought it was odd.  Has anyone run into this before?  Any advice or confirmation that I am not alone with this issue would be appreciated.  If you have any questions, please do not hesitate to contact me.  Hope all is well and have a most blessed day!

Peace,

Pete

Create a Midplane

1st Selection

Cannot make 2nd selection on the same part

Can make the 2nd selection on a different part...

[Anonymous]

Are you attempting this at the part level or assembly level? I can only assume what the problem might be because I'm not in 2015 yet but I'm wondering if, when you're in the assembly level, selection is handled much like a constraint would be (meaning you cannot pick the same part twice). Seems like if it were me, I would open the part file, create the plane, then use it at the assembly level.

Or I could be wrong and you could be attempting this in the part file...

[petestrycharske]

Will,

Yes, I am indeed working in an assembly.  My work around was to create a plane angled about the centerline of my central formed part.  I could also have created a workplane attached to the part, so that was a good idea and I appreciate it.  Just seems odd to me that you can't create a workplane from two surfaces that are in the same part file...

Peace,

Pete

[Anonymous]

@petestrycharske wrote:

...Just seems odd to me that you can create a workplane from two surfaces that are in the same part file...

---

I'm thinking you meant "can't". I agree that I can't see why you wouldn't be able to. Though the image displayed in the drop down menu for that particular tool does somewhat suggest that it uses two different parts. All the same, editing the part file and placing the plane there ought to do the trick. Does 2015 allow for a midplane between angled faces in part files as well? I use the midplane between parrallel faces in part files all the time. Might be cool if I could do the same for angular faces in part files.

Thanks,

[petestrycharske]

Will,

That was indeed a big typo, thanks for catching it.  Yep 2015 allows for midplanes between angled surfaces, which is a big improvement.  I had high hopes that this feature could be used in the assembly, but I it sounds like it won't do what I had hoped.  Thanks for the information and have a most blessed night!

Peace,

Pete

[GarySchmitz3154]

It is hard to tell from the photo if the two surfaces are coplanar, and i am sure they are supposed to be. If there is a rounding error 8 or 9 decimal places out that would cause this not to work. I have found this error when bending large sheet metal parts

[petestrycharske]

Gary,

They are not coplanar and one of the improvements in 2015 is the ability to create a midplane between two angled planes.  However, I cannot create the plane between two planes on the same part in an assembly file.

I am posting this in the Idea Station, so if you think it is a worthwhile idea, please follow this link and give it a vote 

Peace,

Pete

[johnsonshiue]

Hi! This is indeed a limitation in Inventor. Assembly workplane (applicable to other work geometry also) is considered a component, while part workplane is considered a feature. Workplane in assemblied is subject to assembly constraint as opposed to the feature counterpart in part. As a result, when you create an assembly constraint, you cannot select two faces from the same component (subassembly or part).

The workflow to bypass the limitation is to create another assembly workplane (constrained to) the part face. Then, the workplane will be selectable because it is considered a different component.

Thanks!