3D Sweep Error

[Anonymous]

I am trying to create a 3D model of a tunnel that curves 180 degrees and also rises about 10 metres. I have created a 3D sketch of the centre line of the tunnel and a 2D sketch of the profile of the tunnel. I then created a sweep to build the solid tunnel.

However, The solid that is created has "rotated" while it travels along the 3D centre line. This results in the face at one end of the tunnel being "tilted" (I want both ends of the tunnel to be parallel to the x-axis)

I have tried using the TWIST option in the sweep command box but it always comes up with an error. I have also tried using lofts, however the only seem to work on the same plane (Because there is a difference in x,y and z the lofts don't work).

Is there anything I can do?

I have attached the part file for the section of the tunnel that I am having trouble with.

Thank you in advance.

[jeremy_wasserstrass]

Check out the attached file for one way to use a sweep with guide path.

[johnsonshiue · Accepted solution]

Hi! This one can be done easily using Sweep with Path and Guide Surface (see attached). The 3D Sketch path is not tangent continuous. I added a few tangent constraint to make sure the path is at least G1 continuous. After that, I use Path and Guide Surface option -> select XZ plane as the vector guide. The profile rolling will be consistent through out the path instead of following path normal.

Please take a look and let me know if more information is needed.

Many thanks!

[Anonymous]

Hi there,

Thank you for your response. I have a few questions as to how you got it to work. Firstly, what is the meaning of G1 continuous and how did you get the path to be like that?

I have never used the "Path and Guid Surface" option, how does it work?
What constraints did you put on, and how did you know where to put them? I've tried to copy what you've done but it comes up with an error.

Is it possible you can create a screencast?

Thank you again

[johnsonshiue]

Hi Nicolas,

G1 means tangent continuous in CAD. The 3D sketch contains multiple spline curves but at a few intersections, the curves are not tangent continuous. In general, it is better to keep splines tangent continuous so the resultant geometry would be smooth. You want to apply tangent constraints to the spline curves.

Regarding sweep with guide surface, it is a way to control the rolling of the profile along the path. Without using guide surface (XZ plane in this case), the profile will follow the normal vector along the path, which may not yield the desirable result.

Many thanks!

[Anonymous]

Okay, so next time I will keep my curves tangent to one another and create a guide surface that is perpendicular to the desired shape output.

Thank you very much for your help

[inventor1K5NLB]

Hi, I have the same issue, the profile I am trying to sweet keeps kicking out. I am trying to get my curves to be tangent however it will not give me the option on my curves which are drawn using 'curve on face'. How is it possible to get around this? 

[johnsonshiue]

Hi! The Curve on Surface command is best for creating a curve segment connecting two points. There is very limited tangent control when connecting to other curves. To ensure the entire curve be tangent continuous, you will need to either project a 2D curve to the cylindrical face or create the 3d curve entirely.

Here is a simple solution I found by projecting a 2D spline curve to the cylindrical face.

Many thanks!

[inventor1K5NLB]

Hi Johnson, that's actually how I did create the curve, by projecting a 2D curve to the cylindrical face. As you say this works well, but unfortunately I think you have misunderstood what I was trying to achieve as the fixed file you attached is further away than my original attempt. I am aiming for the flat back of the profile to stay flat on the cylindrical surface. Similar to my original file its just the bottom edge flares out slightly. Is this possible to control? 

[SBix26]

I found that your file has some dimensional inconsistencies-- the arc that you used to create the cylindrical surface is not centered on the 811 mm line that defines its endpoints, meaning that the arc is more than 180° and a vertical face attached to the end cannot be tangent to it.  The attached file corrects that issue and successfully generates the sweep for the whole path.

I added the vertical face to the guide surface and wrapped the entire path from one 2D sketch, as shown below.  Since I don't know where all the numbers come from, I don't know how well this meets your requirements.

If I had all the requirements, I would start over, and I definitely would not use a 3D sketch to define the model.  Did you notice that your 3D Sketch1 is not constrained to the origin?  2D sketches are so much easier to work with and so much more robust.

Also, I see that you want the flat surface to lie smooth against the cylindrical face-- how important is that?  It is geometrically impossible for a straight edge profile to sweep along a path and result in a cylindrical face (except in the case of a circular path).  Since the path is attached to one corner of the profile, it looks as if the face of the sweep is tangent to the cylindrical surface at that edge.  If you attach the profile to the path at a different point on the edge (center, for instance), it would be tangent at that point instead of at the corner, but it would still not conform to the surface.

The attached file is Inventor 2024 format.

Feel free to add more detail to your requirements; maybe someone here can figure out how to meet them.

---

Sam B

Inventor Pro 2025.0.1 | Windows 11 Home 23H2

[inventor1K5NLB]

Hi SB, thanks for the file. The 3D sketch is copied over from a much larger file that has relevant constraints hence why it's not constrained to the origin, essentially for this test it didn't really matter but be assured it's relevant in the larger part. I created my 3D curve from a 2D sketch (as Johnson mentioned) and truthfully as I need it to be a consistent single angled line (albeit round a curve) I don't understand how to produce this from a 2D - would you be able to elaborate on your thinking here please? 

The issue here is I originally used tangent profiles to sweep along the curve, but they were not consistent (eg. meant to be 110mm tall, would grow by up to 4mm - not acceptable). I have also tried from the centre, again this did not allow the flat surface to lie smooth against the cylindrical face- this is by far the most important thing. My colleague (CNC operator) who is using my file to manufacture was not happy with my solid model as it flared out (did not conform to cylindrical surface) and created another using other software did it using the method in my file and was able to keep the flat section cylindrical and essentially said I should be able to do the same. So while I agree it seems geometrically impossible, I have seen it done and made..

[SBix26]

---

@inventor1K5NLB wrote:

... and truthfully as I need it to be a consistent single angled line (albeit round a curve)...

---

Can you explain this in more detail?  Is this referring to the 32° angle in your Profile sketch?  I kept that 32° angle in my model but had to use a tangent spline to go from there to the intermediate point and then to the endpoint.

As I mentioned in my previous post, there seem to be some inconsistencies in the defining dimensions and constraints.  I'm not clear what is important.  In the sketch below, which defines the cylindrical surface, the circled measurements show what I think are problems with the definition.  The lower one shows that the arc is more than 180°, and therefore a vertical line at its endpoint will not be tangent, preventing a smooth sweep path.

As far as the profile conforming to the cylindrical surface, Inventor's Sweep tool will not deform the profile; a cut perpendicular to the sweep path will produce an exact replica of the profile everywhere along the path.  If you truly need the profile to be draped over the cylinder, then perhaps the Bend tool is what you need.

Let me know in detail what you're trying to achieve and I'm sure it can be done in Inventor.

---

Sam B

Inventor Pro 2025.0.1 | Windows 11 Home 23H2