How to make those angebars center themselves on the square tube?

[mailswamp]

[JDMather]

Was the angle iron made with Extrude mid-plane (as logical)?
Then simply constraint Mate-Flush the appropriate origin workplanes.

[mailswamp]

I didn't extrude those angles from a center plane. Those angles are standard parts in the database. When you insert them, the inventor asks you how long you want them. Later, they can be extruded to a different length, but I didn't do that.

[Dennis_Jeffrey]

Add a workpoint to th emidpoint of an edge. Then constrain to the workplane you have visible in your post. (Mate Point/Plane)

[mailswamp]

I am not given an option to constrain a point to a plane in the assembly. I am creating a center point but I cannot create dimensions in this environment to see the if the center point is really in the center. Visually it is not

[Dennis_Jeffrey]

Sure you can.....  The workpoint will snap to the midpoint, whether in part or assembly mode.

http://teknigroup.com/Videos/2012Q2/createwkptinassyconstraint/createwkptinassyconstraint.html

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@mailswamp wrote:
I am not given an option to constrain a point to a plane in the assembly. I am creating a center point but I cannot create dimensions in this environment to see the if the center point is really in the center. Visually it is not

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[mailswamp]

The workpoint did snap to the midpoint, but how do I constrain a point to the plane?

That option is not evident in the constraint window. Somehow I got the point to center on the plane but the angle bar stayed in the same place. Also I cannot change the size of the plane.

The point that appeared to snap to the centor visually, can be visible on my drawing and it moved off center somehow. 

[moto748]

When I create a rolled steel section from the Content Centre, I delete the Start Plane, End Plane, and Driven Length features (whilst unticking the "delete dependent sketches and features" tickbox).I then edit the Body Feature, changing the Extents field to Distance, and filling in an appropriate length. Depending on the application I usually set the mid-plane option too.

[mailswamp]

Maybe that can be done for the future angle bar parts but it appears that the developer team needs to look into this problem.

[zma1013 · Accepted solution]

If you insert it as a custom part, you could just add the workplane within the part file itself.  All you have to do is choose workplane option and select the 2 side faces and it automatically places the workplane directly in the center of those faces, which is the center of the part.

Not sure why Autodesk chose to build them the way they did, they really should have made a workplane in the center already or generated it's length in both directions from the center.

I'd like to know an easy way to copy the family of angles in the CC and add my workplane to them instead of creating a custom part.  Would be great to just pull it from the CC with the workplane already in position.

[mailswamp]

True. There is no beautiful solutions so this is the solution.

[mailswamp]

How do I make the workplane that resambles the center of the part stay in the center of that part?

The only way I had achieved that was by grounding the center plane with the  main part. There is a better way to do it, but I cannot put the plain in the folder of the main part in the model tree. How do I make sure the plane doesn't move when I mate it with the other plane without grounding? This is getting pretty complicated. Harder than PTC ProE was...

How do I know if both planes are flush?

Thank you for all the time you spend on me. 

[mailswamp]

PS:

I verified the model with the measure tools.

It looks symmetrical. But Autodesk needs to add more constraints to make it easier to build things symetrical. 

[cwhetten]

You need to create the mid-point or mid-plane (either will work) in the part itself, NOT the assembly.  Open the part in another window just to make sure that you are not referencing any assembly geometry when you create the point or plane.  Then constrain it in the assembly.

-cwhetten

[mailswamp]

I solved the problem by making those bars extrude from a center plane in both directions. Now I found some serious bugs in Inventor. But they are not related to this. SO thanks.