Sweeping feature slow as longer the path

[b_kurt_ch]

Hello

I'm having a problem with a sweeping feature right now that I've never had before.

I'm trying to sweep some sort of rectangular spiral along a cylinder. The path is made up of about 40-50 individual lines created using a 2D and a 3D sketch. When I start selecting the first few lines for the path, everything works fine. The more lines I select, the longer the calculation takes. And extremely exponentially.

10 lines = 1 second

20 lines = 100 seconds

30 lines = 1,000 seconds

40 lines = you don't want to wait.

And what's really weird is that the calculation also increases exponentially with the length of the shape.

Same number of lines, but if you increase just one dimension (See picture X) from 100mm to 1,000mm, it's almost impossible to calculate.

See attachment.

Any idea how to fix?

Thanks and regards

Ben

[kacper.suchomski]

Hi

Create one segment, then duplicate it in the pattern.

[b_kurt_ch]

Thanks for your reply

This is not as easy as it looks. Because the shape is different. See attachment.

Of couse it is possible to cut 45° edge manually, but this is not the goal.

Regards

Ben

[kacper.suchomski]

A few comments:

1. I deleted and re-sweep your file. I measured the calculation time and it was 2-3 seconds. Are you sure you have a computer capable of such work and calculations? Remember that Inventor has its requirements.
2. There is no point in pointing out individual lines. You need to create a 3D sketch; then add the geometry of the necessary arcs to it; then add the lines connecting these arcs. This way you will get a uniform path. The 2D sketches should be invisible.
3. As for the previous content - I didn't mention that it will do itself, only that it is possible. After expanding the array dialog, you can change the calculation method to incremental, so as not to include the full 360 degree angle.
   I won't address chamfering, because this is not the place to complain that someone doesn't feel like clicking. But there's nothing stopping you from marking one more line and then removing the surface (or trimming the body) to maintain a good module.

[b_kurt_ch]

Thanks for your inputs.

OK this is strange. We tested the file also on another computers. Same result. Never had any performance issue till now.

I already tried the sweeping with one 3D sketch. But also with same result.

Have you edited the length by change the two planes from "-2000mm" to "-100mm"?

Because the "short" one works for me as well (some seconds to calculate). The long one needs more time.

My workaround is to create 2 sweepings. One for the left side, one for the right side (both with around 20 single lines). Both has a time of 10-20 seconds to calculate. That's ok for me now.

But I'm curious what happen. Never faced such a problem.

[kacper.suchomski]

I don't have any serious delays.

[kacper.suchomski]

Here is a better method to prepare the path:

[kacper.suchomski]

There are more things to improve in general.

The dimensional constraints in the first sketch are not healthy. They should be duplicated in pattern, and if they cannot be duplicated, they should have geometric equality constraints - there is no reason to put a pile of dimensions there.

Also, 2 larger dimensions are unnecessary - since all arcs are concentric it is enough to apply a horizontal constraint to the endpoints.

[b_kurt_ch]

Hi Kacper

Thanks for your great effort!

I did exactly the same as you in both videos. We tried it on 3 different computers. Maybe not the newest one. But with 32GB RAM / 20 cores at 2.5GHz each, I don't think that should be the cause of the lag.

Doing it with a single 3D sketch shows the same result.

Your comment about the sketch is correct. But the design is made for flexibility.

In this example, all arcs are identical. But we need the ability to adjust. It could be that one arc needs to be 20 degrees, another 30 degrees and so on.

I guess, this sketch should not be the source of the error. It seems, it's the sweeping itself.

Because another strange behavior is:

Sweep 5 lines. Press F6 to center the model in ISO view.

Sweep 6 or 7 lines and press F6 again is a completely different center point of the model. It seems as if Inventor is enlarging a line in the background significantly more than it should be.

My guess: On your computer is also this behavior different? 😉

[johnsonshiue · Accepted solution]

Hi! I guess it is a combination of the hardware and the geometric complexity leading to the slow compute. Rebuild All seems to work relatively fast on my machine.

Another workflow to consider is to create Sweep Surface instead. Edit the Sweep profile sketch and select the inner curves and change them to Construction lines. Then sweep the profile along the same path. After the Sweep surface is created, use Thicken command to solidify the surface. It seems work work twice as fast compared to the Sweep as a solid body.

Many thanks!

[b_kurt_ch]

Dear John

Thanks for your answer.

The sweeping with faces is a good idea. I tried it and it works. Much faster than before.

If the total length is about 4300 mm, the calculation time is now about 6-7 seconds. That's OK.

Only the edges are not so nice because sweeping with faces does not automatically cut interference. See attachment.

But for this case, it's not that important to have a perfect looking model.

Thanks and regards

Ben