How to stop the sweep function from rotating the sweep profile about the axis of the sweep path?

[Snelso91]

I am currently trying to cut out a circular hole for a wire, as well as a perpendicular slot/channel that reaches from the circular hole to the surface of the body, so that the wire can easily be moved in or out of the circular hole.

I have a 3D sketch which contains the sweep path of the wire, and this path is comprised of a spline, 2 straight lines, and an arc:
Top view (starting point is at the bottom right)

Rear view (from behind the starting point which is at the top left):

Here is the sweep profile for the wire hole, which contains an arc at the bottom for where the wire sits, as well as a vertical rectangle above that to cut out the slot to the surface of the body that the hole is being made in:

If I sweep just a circle along part of the path, or I use the pipe command with the correct diameter, then the result is as expected which is that a circular body is formed that is always perpendicular to the sweep path.

However, when I perform the sweep with the sweep profile previously shown instead, the sweep profile remains perpendicular to the sweep path, but the sweep profile also rotates, with its rotational axis being the sweep path. This means that the slot that is supposed to remain vertically upwards is now rotated over sideways as the sweep moves along the path, which is not what I want.

You can see that the side walls of the swept profile have now rotated clockwise about the sweep path (when viewed from this angle) and are no longer parallel to the 2 vertical faces (highlighted in blue).

I have tried to use guide rails or guide surfaces with the sweep tool in order to keep the walls vertical, but unfortunately neither of these solutions gives me the result I want.

If I use the flat top of the body that is being cut into (which is perpendicular to the vertical side walls I am trying to cut) as the guide surface, then the walls are now vertical, but the sweep profile is no longer perpendicular to the sweep path (see the original pipe extrude sticking out from face of the sweep as they are at different angles)

I could instead use the surface sweep command to create a top surface that is the same as the result of the above sweep command. This would in theory then undulate up and down to remain perpendicular to the sweep path, unlike the flat planar surface in the above example.

If I then change the guide surface of the first sweep to this new surface, then I get a result that is close to what I want, but it is not identical to the basic sweep/pipe command at the bottom. The angle is different relative to the sweep path (see the pipe extrude sticking out at the bottom in darker grey shading)

If I use the edge of the surface sweep as a guide rail for the sweep command, and select the "scale" mode, then the created body is not the right diameter at the bottom (it is smaller than the original pipe command in dark grey)

If I change the mode to "stretch", the width is now correct, but the height is still wrong (the bottom of the pipe command in dark grey is still lower than the bottom of the sweep):

Therefore what I want is to create the same shape as the normal sweep tool (i.e. keeping the sweep profile perpendicular to the sweep path and not distorting/stretching the profile), but to simply eliminate the rotation about the axis of the sweep path.

In other words, I want to keep the 2 axes of rotation that allow the sweep profile to rotate up, down, left and right in order to remain perpendicular to the sweep path, but I want to lock the 3rd axis of rotation which rotates the sweep profile around the sweep path axis.

How can I achieve this in fusion?

[jhackney1972]

Please attach your model.  You have a lot of screen captures but they do not allow the Forum users to find your issue.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[Snelso91]

My apologies.

I've now created a simplified cutout version of the original assembly (since it was quite large) and put only the parts relevant to this problem into a separate fusion file, which I've attached.

The bodies under the top level component represent all the different variants I discussed in my original post, and you can find the features that generate them in the timeline.

The sketches I was referring to in the original post (and which are used to generate the sweeps) are under the "Wire" subcomponent.

Thanks in advance for your help with this issue.

[davebYYPCU]

Add more profiles to the existing Surface > Sweep.

If you want a channel cutter, I would convert to solid (Patch both ends, and Stitch)

and Combine > Cut with it.

Might help....

[Snelso91]

Thanks for the suggestion. I tried it, but unfortunately it doesn't give the result I'm looking for, as the final solid body (formed from the stitched surfaces) is identical to the "Sweep Guide Plane" body that I already made using the solid sweep function (if you hide or unhide each body in turn you can see that nothing changes so they are the same).

This kind of result is not what I want because although the side walls are vertical relative to the channel, the profile is no longer perpendicular to the sweep path. For example in the below picture, the original pipe/circle sweep (highlighted in light grey) is following the sweep path at the correct angle, whereas the sweep guide plane body is sticking straight up and so is no longer perpendicular to the sweep path.

I've attached this new version of the test file so can you see what I have described.

It is important for the swept shape to be "leaning" over at this angle (i.e. remain perpendicular to the sweep path) because the actual sweep cut I will be doing will only be partway along the total path (leaving a hole in the middle for the wire core of course). Because the wire is soldered/fixed at the end of the copper core (on the left of the photo) in order to remove the wire cleanly, the cut needs to be tilted over like this (cut using the "sweep no guides" body), or possibly tilted over even further.

Whereas if you have a completely vertical slot (cut using the "sweep guide plane" body) it will be much more difficult to tilt the wire up and out of the slot from the right hand edge (with the insulation):

So when I say I want vertical walls, what I'm referring to is the first picture where the walls should be vertical if looking in a plane along the sweep path. In other words they are perpendicular to the sweep path. However they should not be tilted/rotated over to one side like using the sweep no guides body gives (see below).

To be specific, what I want is a result that is the same at the "sweep no guides" body, where the cross section of the swept shape (i.e. the sweep profile) remains perpendicular to the sweep path at all times. However, I do not want the sweep profile to rotate around the axis of the sweep path.

This rotation can be seen in this picture where I used the sweep no guides body to perform the cut. The cut is clearly tilting over to the left compared to the vertical cut walls in the middle. In other words the cut is rotating counter clockwise with the sweep path as its axis of rotation.

I want to keep the same sweep shape as the sweep no guides body, but to simply get it to not do this rotation about its axis as it moves along the sweep path. From what I have found so far, none of the other bodies/sweep options can create this desired result, because either the shape is distorted compared to the sweep no guides body or the angle is wrong (either it is rotated about the sweep path, or it is no longer perpendicular to the sweep path).

If this is not at all possible using the sweep tool, then perhaps I need to look into using loft?

Although I was trying to avoid that as it would become more complicated such as needing to provide a second profile at the other end to loft to (whereas sweep only needs 1 profile) and guide rails to get it to follow the sweep path.

[Josef_A_K_]

Hi, I've done it with sweeping on a path and additionally with "Führungsfläche" (I worked with German software).

You will see it in the picture, hope it works also on your site.

[Snelso91]

Hi, I tried to copy what you did in the image by changing the guide surface (Führungsfläche) to the face of the crimp connector, but it hasn't changed anything and the result is the same as the "sweep guide plane" body in the "sweep issue v5.f3d" file in my previous message.

I explained in my previous messages that the shape of this body is not what I want as it makes the sweep profile no longer perpendicular to the sweep path, so I don't think is a solution unfortunately.

Please let me know if I have missed something.

For example, what is the purpose of the "second sketch on the end" in the left area of your picture?

From what I can see it doesn't appear to be used in the sweep command, but perhaps I am misunderstanding?

[davebYYPCU]

Ok, I think, try Sweep solid, using the black tube, in the vertical direction.  You may have to add draft to that result for the bent end,

or revert to a Loft, using the plane on the end of the black pipe, for a second profile.

Might help….

[Josef_A_K_]

Hi Snelso91, so the sketch on the end of the path was a test to use "Erhebung" (in German) instead of sweep. This was not successfully, but indeed changed a sketch from You, didn't think that there is a treason of success.

I tried it again, and You are right it doesn't work with your sketch- what else did I changed:

I went into your sketch "wire path" and delete all the tangential constrains and added all tangential constrains again. May be you had a constrain on the "green" line of the path, instead on the blue. It works.

I send you the result. Hope it fits.

Greetings from Germany

[davebYYPCU]

Solid Sweep appears to work Ok, black tube is too short to reach profile, but easy fixed.

Might help....

[johnsonshiue]

Hi! Please bear with me if I repeat the technique. For this particular case, you will need to create a Ruled surface based on the Sweep path in the desirable direction. Select the surface as the guide surface. Please take a look at the attached file.

Many thanks!

[Snelso91]

Thanks, this is a great suggestion!

I tried the solid sweep using a body called sweep insulation that is slightly bigger than the black tube (for clearance) in the vertical direction and it is very close to the result I was looking for (although not exactly the same because of the lack of the angle).

However its real use comes from the fact I can sweep the body across an arc, which simulates what would happen when the wire is pulled up and out from the right hand end with the crimp connector.

So although this is technically not the exact solution to my original question, this is arguably a more optimal slot shape than the one I was aiming for originally given its intended purpose, so it's a good solution nonetheless.

In the attached file you can see the result of cutting out a solid sweep vertically and then followed by another solid sweep following an arc with its centre coincident with the centre of the soldered piece of wire (arguably the axis of rotation when pulling out the wire from the other end).

If you want to see just the vertical cuts, then you can go back 2 steps in the timeline.

[Snelso91]

Hi, unfortunately the shape in the file you attached is the same as in my previous reply to you (post #7), so it still has the same issues.
I have found some alternate solutions now so I don't think we will need to pursue this specific attempt at solving the problem any further, but thank you for your efforts nonetheless.

[Snelso91]

Hi, this is exactly what I was imagining when I was originally thinking of the shape that I wanted, thanks for letting me know about this solution!

In other words the shape is exactly the same as the default sweep with no guide rail or guide plane, but is no longer tilted/rotated over to one side and is instead vertical.

However, there is one problem - although this sweep with ruled guide surface works properly when the sweep path is only the first straight line and the spline, if I change the sweep path to include the full path in the "wire path" sketch, then the sweep fails with the error:

"Error: The sweep would not create a valid result.
Try adjusting the values or changing the input geometry."

If I use the full path but set the distance ratio to 0.88, then the sweep is generated without errors, but the shape is clearly distorted (highlighted in blue) and not a smooth continuation of the previous part of the sweep.

Please see the attached file for further details.

I checked the underlying sweep path in the wire path sketch but I couldn't see anything obviously wrong with it that could cause these errors, and it is also a fully defined sketch.

Do you know how I can fix these errors?

[johnsonshiue]

Hi! Many thanks for sharing the updated model! I took a quick look. I am sorry I think the particular Ruled Surface may not work well for this Sweep. Instead of using the Ruled Surface, the YZ plane should be selected as the Guide Surface. Edit the Sweep and select YZ. It should work better for you.

Thanks again!

[Snelso91]

Hi, unfortunately using the YZ plane as a guide surface doesn't give the result I want. The angle of the sweep is wrong and the bottom of the sweep is distorted compared to the perfect/desired result using the ruled guide surface (see attached file).

Is it possible that there is some bug with the sweep function with guide surface where it cannot be used with a sweep path that is a 3D sketch with a combination of a spline, arc, and straight line that are all tangent to each other?

[TrippyLighting]

I am not entirely sure what geometry you want to end up with, but you were on the right patch with the Ruled surface.

Sweep isn't the right tool for this.

[Snelso91]

Thanks for the suggestion on using thicken, this produces the shape I want for the wire core channel cut.

To clarify, my goal has been to create 2 cuts, one which runs the full length of the path in the "wire path" sketch, and is a smaller diameter. This is to create a channel for the uninsulated copper wire core to fit into. Let's call this cut (or the bodies associated with making that cut) the "wire core channel".

The other cut is one that only runs up to a point that is partway along the spline, and is of a wider diameter in order to fit the wire insulation, as it does not run the whole length of the wire in order to avoid interference with other components in the assembly. Let's call this cut the "wire insulation channel".

Your example of using the thicken command, boolean combined with the existing pipe sweep body gives the correct shape for the wire core channel, and so do some other options such as using a sweep with a YZ guide plane, combined with the pipe sweep, or using a vertical solid sweep (see attached file for these different methods and their bodies).

The solid sweep does produce a rounded top instead of a flat one, but I don't care what shape the top of the body is, because it is the vertical side faces and the bottom arc face that will be cutting the channel into the capture plate component. So these 3 methods are all equivalent for this purpose.

However, the thicken command does not work for creating the wire insulation channel shape that I want, because it creates a cross section that is not perpendicular to the sweep path and is instead aligned vertically. The other methods I mentioned also have this problem. In addition, the thicken command can't select partway along the surface body with a ratio (e.g. the first 75% length of the body) like you can with a sweep command where you input the length ratio.

So these two issues make it not suitable for the wire insulation channel cut.

So far the only way I have found to make the correct wire insulation channel shape is to use Johnson's suggestion in post #11 to use a ruled surface as a guide surface.

Since the ruled surface is just a vertical line that follows the curvature of the wire path sketch, I can also generate the same surface body by doing a surface sweep of a vertical line along the wire path.

There is a slight advantage to doing this which is that I noticed that the ruled surface was a little buggy and would give errors if you set the height to a number that was too large, whereas the surface sweep of the vertical line didn't seem to have any issues. I've included both in the file for reference.

However, the issue with the sweep using the ruled or swept surface as the guide surface that Johnson suggested, is although it works fine for the wire insulation channel which only extends partway along the wire path sketch, if I try and extend this same sweep by changing the length back to 1.0 and selecting the whole wire path, then it gives "The sweep would not create a valid result." error.

So, although I now have methods to create the two different channels exactly how I wanted, what I was looking for before I wrap up the discussion was if there was a way to use the same method with different inputs to create both the wire core channel and the wire insulation channel?

For example, if it did not give an error, then I was expecting the sweep with swept guide surface to also create the same shape that I wanted for the wire core channel, in which case I could use this tool for both channels.

You can see in the file that a normal sweep with no guides works fine when using the whole wire path, so why would the sweep with swept guide surface not work given that it is the same cross section, just not rotated off to one side?