How to sweep/loft this geometry

[stephenmcd74]

Good afternoon

I have been trying various sweeps and lofts to create some geometry, but can't get anything to work.

Please can anyone help me with this??

Ok so I have the solid which you see below (ipt. file attached).

To explain, please imagine a mobile horizontal axis. One end of this axis is connected to the vertical (in this case y) axis, and so the new axis can pivot around the y axis, but its point of attachment can also slide up and down the y axis. 

There is a green "guide" line (3 axis sketch) visible along the leading edge of the "apron". The mobile axis (always remaining horizontal and still connected to the y axis) should move along this guide to slice away the lower portion of the part. As the mobile axis moves towards the centre of the part (YZ plane) its point of attachment to the y axis will slide downwards.

I have tried sweeping a sketch with 2 guide rails, as well as using sketches for the start and end of the modification (see last image below) and doing a loft, but none of these works.

I would be very grateful if anyone can tell me how to do this.

Thanks a million

Stephen

[Frederick_Law]

Move cut to center of curve

[stephenmcd74]

Good afternoon

Thanks for this.

However unfortunately that isn't what I need. Sorry, maybe my explanation of what I am trying to do isn't very clear, but maybe read it again?

If the modification is correct, and if I then create a vertical plane between the y axis and anywhere on that modified face, and start a sketch on that new plane, the lower line of the cut section should always be horizontal.

In the image below I am looking directly at that end face, and you can see that the bottom line is not horizontal. Rather, the cut is only horizontal in the centre where you have started from.

Thanks

Stephen

[stephenmcd74]

Effectively, in your version the 2 outermost faces of the sweep are parallel with the central face from where the sweep begins (see below).

I would need that as the sweep progresses, the face being swept is always remaining both vertical (so passing through the y axis) and radial (so sliding up/down the y axis), so its orientation of the face is constantly changing along the sweep.

Thanks again

Stephen

[Frederick_Law]

So, change the options in the sweep and see if it give you result you need.

I read your post 5 times.

Don't think I'll get anything more if I read it again.

[johnsonshiue]

Hi! This is a very interesting Sweep challenge. To keep the cut horizontal relative to Y axis, you need to use Guide Surface Sweep (XZ plane). After the cut is made, Delete Face/Heal is needed to remove some faces. It is because the side faces are not perpendicular to the path. The Sweep cannot clean up the detail geometry. Please take a look at the attached part.

Many thanks!

[cadman777]

Hey Johnson,

I tried that on my version of Inventor, then tried it in Rhino.

See attached failed attempts in both apps.

Does IV2023 do it correctly like the horizontal lines show?

Notice that the cutting surface is not parallel (fully contacting) the middle of the 3 lines.

Note:

- I made the surface differently b/c it was too much trouble trying to duplicate the OP's model. So I just did a 'make-do' part for doing the cut.)

- The '-3dm' part is the Rhino part imported into Inventor as a STEP file.

- The other part is native Inventor.

[WHolzwarth]

Another approach from here (2023 IPT). Too late i noticed, that the initial file is 2020.

[johnsonshiue]

Hi Chris,

This particular case would be extremely difficult to do in 2015 and earlier where Guide Surface Sweep was not allowed. Without it, there is no way to control how the profile orients itself along the path. It would depend largely on the normal direction along the path. However, such normals are not editable by the users.

The way I solved this problem is to use a Guide Surface Sweep (XZ plane as guide, equivalent to Y-axis). The resultant cut face remains horizontal at each cross section. Please take a look at the attached STEP file.

Many thanks!

[stephenmcd74]

Hello there Johnson

This is very nice attempt. However sorry but this is still not what I need.

Here is a different way of explaining:

Attached is another file, shown in the image below. I have added 7 axes. All of these pass through the y axis of the part, as well as a point on  the 3d sketch1. These axes are 3.75° apart (see sketch 10). Imagine there were an infinite number of these axes along the 3d line in sketch 10 - all passing through the y axis: this would create the cutting surface I need. 

Can you find a way to create this sweep?

Thanks again for your help

Stephen

[johnsonshiue]

Hi! I guess there isn't a great solution in Inventor for this case. The closest I can get is by using Ruled Surface. Please take a look at the attached part. You may need to tweak the angle of the Ruled Surface.

Many thanks!

[blandb]

I'm having a difficult time trying to understand what you are looking for, but if you are needing a surface that essentially passes through the vertical Y-axis, but curves to the lip, can you just make a sketch on an origin plane, then draw a line. Next, loft that line to the edge desired (I had to switch the  transition connection points) but made a surface that will go through the edge and the axis. I then split the solid with that surface. Next created a ruled surface with a Z vector, and then did replace face to make it flat from the side view....See if the attached is what you are trying to accomplish?

[cadman777]

Thanks Johnson!

You are correct.

When I attempted to use 'guide surface' it gave a very strange result!