topic Re: Sweep not following multiple paths in Fusion Design, Validate & Document Forum

Sweep not following multiple paths

lkeays — Sat, 18 Jul 2020 11:33:59 GMT

Hi - trying to CNC a simple picture frame and I want to sweep the outside borders.

Made my design with a simple corner - then mirrored left, then down.

Sketched from "3d Geometry" is the result here - but it's still 4 separate splines. I've tried everything to "join them" but can't figure it out after searching and searching.

Sweeping just "rounds up" instead of following the path. What am I doing wrong?

Re: Sweep not following multiple paths

beresfordromeo — Sat, 18 Jul 2020 12:27:03 GMT

Hi @lkeays

I have had a look at your file and I am trying to understand what you are trying to do so apologies if these seem like silly questions.

1. Why are you using the form tool for this exercise.

2. Do you know why there are so many errors in the file. In particular what is the purpose of the two CutPaste operations.

Re: Sweep not following multiple paths

beresfordromeo — Sat, 18 Jul 2020 12:50:39 GMT

So one way of seeing why a sweep might fail is to sweep any single aspect of it using the surface environment.

The curvature in the top section of this frame is too tight to accommodate the size of the profile you are trying to sweep and would result in an intersection of some kind.

You can get around this by changing your outside (backing?) shape if that is at all possible or profile (frame?) you are trying to sweep. I won't go any further right now because the intent of your design will determine what approach you might take for resolving these issues.

Please bear in mind that even if this sweep were to succeed machining this would be a tricky operation, it would require a long bit with a very small diameter and depending on the material you are using could be impossible.

Having said that it is very likely I have misunderstood what you are attempting to do so please feel free to ask any further questions or point out why I may be incorrect in my assumptions.

Re: Sweep not following multiple paths

mmharris — Sat, 18 Jul 2020 13:41:25 GMT

a few thoughts

1) I am not an expert

2) start with a simple experiment if you are having problems

3) always fully define sketches

the ends of the paths of a sweep might have to be tangent

see my test bodies added to your sketch

step 1 a simple profile kinda like yours sweeps around a circle easily

step 2 would not sweep around mirrored splines till I added tangent constraints to joints

swept fine

step 3 think

for your shape I suggest creating 2 lines at 90 degrees and 1 spline extending past both

create your profile and sweep then cut off the solid at the 90 degree line and mirror 2x

Re: Sweep not following multiple paths

beresfordromeo — Sat, 18 Jul 2020 13:48:18 GMT

Hi @mmharris

Although I appreciate the attention I am not sure that you were intending to reply to me rather the person with the issue @lkeays.

Re: Sweep not following multiple paths

mmharris — Sat, 18 Jul 2020 14:35:32 GMT

split the path as often as you have to avoid sharp inside corners

mirror body to avoid self intersecting sweep

BUT as was pointed out;

if you plan to cut this, "sharp" inside corners are limited to the radius of the cutter or bigger

Re: Sweep not following multiple paths

mmharris — Sat, 18 Jul 2020 14:37:57 GMT

Sorry,

glad your sense of humor is working

please see "1 i am not an expert"

Re: Sweep not following multiple paths

laughingcreek — Sat, 18 Jul 2020 16:29:17 GMT

The very first problem is conceptual. the profile is not perpendicular to the path-

the profile sweep sweep around the path maintaining the relative angle to the path it started with. the results are usually not what is desired.

one way to make the profile perpendicular to the path is to use "plane on path" and put the profile sketch there.

you can see this in my attached file

the next bit to realize is that when a profile sweeps around an inside curve that is to tight, the resulting shape will self intersect. if you offset the path (I used surfaces for this. the geometry is better than when you offset a spline) you will see that the inside curves eventually just form a sharp angle. sweep can't handle that.

interestingly, sweep can handle sharp corners in the original path. in that case it knows to form a miter. go figure.

anyway, the attached is kinda hacky, but have a look and see if you have questions.

Re: Sweep not following multiple paths

lkeays — Sun, 19 Jul 2020 10:00:28 GMT

Thanks, I understand your tip about testing it first on a simpler form. I understood that the splines needed to be tangent - but I failed after quite a lot of attempts in making them so. The points are "on top of each other" so how can you select the one below? Even if I move one of the splines, it doesn't want to converge.

I used mirrors because it's the easiest way to have a perfect path on all sides. Hmmm

Re: Sweep not following multiple paths

lkeays — Sun, 19 Jul 2020 10:02:28 GMT

Hi,

Thanks for the help. I am still very junior in fusion - so I wouldn't know why so many errors - I mean this file is the result of probably 2 hours of intense frustration of not being able to do it 😉

I used forms simply because nothing else worked... But that might be my ignorance...

Re: Sweep not following multiple paths

lkeays — Sun, 19 Jul 2020 11:02:04 GMT

Thanks for that! I carefully followed your timeline and I think I got it. If I summarize it in "instructions" (for myself to remember):

Work on a simple corner that you'll mirror later
Create a plane along the path (so you have a 90o angle plane to your path)
Extrude the path
Surface offset path to make a "smaller similar path inside"
Create your "sweeping shape" within the 2 "walls" of inside the offset
Fillet the very sharp angle so it's a curve (of the inside offset path wall)
Sweep (notice the sweep will flow extended to the area of the "corner" you'll later mirror
Split the surface that it's actually flowing over that area (it will create a nice sharp "slice" for the mirror later)
Delete the bits flowing over the "mirror" area
Mirror left, then mirror down
Combine the 3 mirrors (why?)
Delete bits left over
Be happy.

Re: Sweep not following multiple paths

lkeays — Sun, 19 Jul 2020 13:56:32 GMT

May I ask a question? I've tried replicating "from scratch" and I got almost to the end but my sweet stops before the fillet part. Tried many ways but can't seem to edit the red spline or create an extra spline at the end to follow and coincide it . What am I missing? Thanks.

Re: Sweep not following multiple paths

laughingcreek — Sun, 19 Jul 2020 14:30:26 GMT

I don't have time to get in depth ATM, but maybe later today. in the mean while-

-for the immediate problem, use the edge of the surface for the path, not the line in the sketch (either long left click to get a list of possible selections when things are on top of each other, or turn the sketch off)

in the original , I created the offset to see where the path would form a sharp angle that would foul the sweep, then put a radius on it so it would go around it smooth. You can see the effect in th epic above, as the sweep doesn't conform to that curve on the upper part when using the inside path. trade offs have to be made (or different tools)-

Re: Sweep not following multiple paths

beresfordromeo — Fri, 24 Jul 2020 07:05:26 GMT

Hi @lkeays

Do you still need help with this file? Please let me know if you do and if you have made some changes please upload your latest version so we are working from the same place.

Re: Sweep not following multiple paths

lkeays — Fri, 24 Jul 2020 18:02:51 GMT

Appologies for the silence. I understand your approach and at this point, I decided to change approach to make it simpler, - the size of this would have been very small for my CNC machine. So I just filleted the border.

Thanks a lot for the help!