Sweep across multiple line segments

I recently upgraded to the latest version of Shapr3D for iPad and am experiencing a problem that I didn’t have in the past. I have created a sketch of a spiral that is composed of multiple arcs, and then use the Sweep tool to create a solid body.

If I now try to make a tapered spring by selecting one end and moving it upwards, then only solid body related to one of the arcs moves as shown below:


I don’t think this happened in older versions and I wondered if anyone can point me in the right direction?

Thanks in advance

Hi Fortuna,

Welcome to the forum.
I don’t think the sweep behavior has change recently.

You have to create a spline instead of arcs, this is the only way so get a single surface body when sweeping. Then, you will be able to move and bend the whole shape as expected.

Here is a quick and dirty video showing it.
Hope it helps.

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Thanks so much for your quick response, and the video provides me with a solution!

I still do wonder whether something has changed in Shapr3D (or I’m misunderstanding the sweep function!). In the past I used this video to achieve the same effect:

In that you can see that the spiral is made up of multiple line segments, however, after applying the sweep to each segment the new solid body seems to be able to be stretched as a single entity. I’d be interested in your comments?

Many Thanks

Hi Fortuna,

you are welcome.

Obviously something has changed, as your video proves it. Do you know which version was used?

I’m currently on Monterey 12.2.1 so the oldest Shaprd3D’s version I can run is 5.50 , late January, and the behavior is similar to 5.100.
I may install Big Sur on a virtual parallel machine to go further back in time, (I need to test non regression on other software), but the ones who knows what and when it has changed are Shapr3D’s team :grinning:

Clearly the old behavior was way better: when we sweep along tangent arcs, we wish to create a single surface without edge, as it is already the case along aligned line segments.

I have a feeling that I was using v4.12, but it definitely wasn’t at v5. You are right the old behavior is much better :slight_smile:
How do we go about reporting this regression to the Shapr3D team?

Hi @Sebestyen

it seems that the sweep behavior has changed at some time.
When we sweep along aligned segments or along arcs of the same radius, it creates a single surface body as expected
But when we sweep along tangent arcs of different radius, it creates an edge separating two surfaces, which does not allow to bend the whole shape (see the first post of this thread).

@fortuna shared a video showing this was not the case in earlier versions of Shapr3D.
[Sweep across multiple line segments - #3 by fortuna]

Is there a good reason for the change or is it a regression? The previous behavior was clearly way better.

Thanks in advance.

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Hey @PEC

Great observation, this is a question that comes up rather often and it has a quite simple answer.

The reason behind us changing to have an edge at the start of an arc or spline is because when we introduced our “Drawings” tool, we had to make sure that the curve can be annotated separately. Because of the kernel itself, if the swept line was one continuous line, you couldn’t have annotated it in Drawings.

Keep in mind, that this doesn’t mean that the swept part is consisting two bodies, as you can see that upon sweeping along the curve, it became one, called Body 01 in your example.

Thanks Sebestyen for your prompt and detailed answer.
I understand the reasons why you did it that way.
So if someone doesn’t want the edge, he should use a spline for sweeping.

Be aware that at every sketch change, whether it’s a line-to-spline or a line-to-curve, there will be a line.

If someone doesn’t want an edge, the best way is to make it disappear if you wish to take a screenshot is to use the built-in Screenshot tool and turn the edges off, or use the newly released Visualize tool.

this is how I was able to edit the spiral


you should also have a look at (Tapered thread - #2 by Robert)
which is for me the fastest and easiest way to go (thanks @Robert).


No problem :wink:



Just a note about this method. It works if you have a small number of points on the spline (which makes the spiral less accurate), however, if you try to make the spiral accurate with many points then you will get an ‘Edge transform failed’ error message when moving the end of the solid body. Seems like I will have to use one of the other methods that people have kindly provided.
Thanks for all your assistance