how to keep square and flat extrusion when angles

[serpennica]

Inventor 2023

when i create an extrusion or sweep, I am unable to keep the face's square to origins or each other, both at the same time. Is that possible?

i have 3 configurations in the example. what I am trying to do is measure the surface top and surface side to each other and get 90deg, also measure the top surface to an origin plane to get 90deg and side surface to origin plane to get 90deg. I would think I could get 90deg for all when measuring but I get 90.03 etc....deg.

I am trying to constrain the sketches in different ways but have not found right combination.

Extrusion 1, constraints are vertical line to vertical projected origin and horizontal line to projected origin.

Sweep1, no difference, just horizontal constraint.

Extrusion 2, constraint parallel to projected origin. this is the best, but still have side not at 90deg to origin.

By setting up the different constraints I am trying to get the extrusion square, but any configuration always results in an angle not at 90 deg.

thank you

image 1 is face to face,   image 2 is face to origin

[CCarreiras]

Hi!

Maybe using Frame Generator?

[Preston_Reed]

@serpennica that geometry doesn't work, it doesn't matter if you use loft or sweep.  As soon as you change both the x and y of the end point it will not be square.  Frame gen would work but if you are wanting to follow this path the 2 end points need to face each other. 

[kacper.suchomski]

Hi

1. Create a plane perpendicular to the sweep axis (perpendicular to the extrude direction).
2. Create a sketch of a rectangle/square.
3. Extrude / Sweep.
4. Trim the faces to the reference surface.

You can't cheat math.

[pcrawley]

I agree with all the above - but are you are trying to work out why your approaches don't work?

If you cut a piece of box section steel at (say it's 50 x 50, with a 45-degree cut), then measure the length of the cut face, it won't be 50x50.  It should be about 71x50.  You've sketched the cut face - so your sketch is not perpendicular to the sweep path, but you are using the dimensions of the uncut shape.  In pictures, it looks like this:

If you create the section sketch (5x8?) at point (1) perpendicular to the path, extrude between the start/end planes, then zoom in to where you've drawn your sketch (2) - you should see why you can't get a 90-degree angle with the measure tool on your model.