Autodesk Inventor

[#1]

I am having difficulty aligning the profile for a sweep feature.  I need the profile to be normal to the path, but aligned veritically.  In other words, the rectangular profile should remain "plumb" along the entire sweep.  Is there a simple way to do this?

I have shared the sample files, trying to use the profile in two different ways, through Dropbox (they are too large to upload).  I am using Inventor 2013.

https://www.dropbox.com/sh/n4vjgiv426a85sx/jnBf0O_yUQ

Thank in advance for your help.  A bit of an urgent situation... so please help!

[#2]

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trobinson.hitech wrote:

 (they are too large to upload).  I am using Inventor 2013.

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Sounds like you need to Sweep with Guide Surface.

Find the red End of Part marker at the bottom of your feature tree.

Drag the red EOP to the top of the browser hiding all features.

Save the file with the EOP in this rolled up state.

In Windows Explorer right click on the filename and select Send to Compressed (zipped) Folder.
Attach the resulting *.zip file here.

[#3]

Thank you for the response.  I derived parts with the necessary geometry to creat acceptable file sizes.

I need to understand how to solve the sweep in both examples.

Thank you for the help.

[#4]

I attempted to use the "Guide Surface" but clearly do not fully understand the concept.

I get the error:

   Create sweep feature failed
     SweepSample_R1.ipt: Errors occurred during update
       Sweep4: Could not build this Sweep
         The attempted Sweep operation found a sweep path which is not tangent continuous. Try with different inputs.

[#5]

Can you include a screen shot with sketches on for those of us with earlier versions?

[#6]

See screen shots below.

The path is a along the curved surface, created with a 3D sketch from interecting planes.

[#7]

if I understand correctly you want the sweep to follow the path, but remain verticle, not like sweep actually does. It normalizes it to the path. You may need to repeat your sketch at key path points and then loft from sketch to sketch using the path as a rail. I had to do this myself once along time ago and at the time was the only way i could figure out how to do it. Hopefully someone will know an easier way.

[#8]

The spline faces in your SweepSample.ipt are extremely heavy.  Those causes slow performance and a huge file size.  I would recreate the entire model using lines and arcs so that the final body can contain analytic geometry as much as possible.  I simplified your model and attached four IPTs that show different sweep options.  Note that the path consists of four curves that are not smoothly connected (i.e., not G1-continuous).

1. SweepSample_perp.ipt: The perpendicular sweep (default sweep type) can take non-G1 path and make miter joints as necessary.  The cross sectional profiles are always perpendicular to the path.  This sweep type minimizes the profile rotation around the path.

2. SweepSample_surf_normal.ipt:  In surface normal sweep, the profile orientations are controlled by normal directions of a guide surface.  The following two conditions are required to make the surface normal sweep successful:

    (1) The path must be smoothly connected (i.e., G1-continuous).

    (2) The entire path must lie on the guide surface.

You could have multiple segments in the path and multiple guide faces as long as the above requirements are met.  Since the path in this model is not smooth, I created a surface normal sweep for each path segment.  Problem is that the user needs to manually take care of miter joints between adjacent sweeps, which is not easy.

3. SweepSample_parallel_A.ipt:  All cross-sectional profiles are parallel to each other.  This model contains analytic geometry only: planes, cylinders, and cones.

4. SweepSample_parallel_B.ipt:  The same as above, except the orientation of the profile plane.  This is the simplest model you can get, containing only planes and cylinders.

Let me know which orientation among the four models is most suitable.

Glenn

Autodesk ShapeManager Development