topic Re: Sweep Problem in Fusion Support Forum

Sweep Problem

ahmed_afathalla — Fri, 27 Jul 2018 18:26:53 GMT

Hello,

I'm trying to make a slot for the lens in the glass frame as shown in the attached pictures using sweep (cut), sweep path is the outer curved path of the frame as shown, sweep is working fine to the point where the frame curved down then it refuse to sweep showing deviated "unsweeped" path, any solution?

Re: Sweep Problem

ryan.bales — Fri, 27 Jul 2018 19:45:35 GMT

Hi @ahmed_afathalla,

Hard to say without seeing the file. Have you played with the orientation?

Re: Sweep Problem

ahmed_afathalla — Fri, 27 Jul 2018 21:02:06 GMT

Hello Ryan,

I'm not sure what do you mean by changing orientation could you please specify, I have tried so much combination but still was not able to make that simple sweep to work all the way till the end, I have no problem sharing the file please let me know how I could share it with you as I'm still new here using that forum.

Thank you,

Ahmed

Re: Sweep Problem

ryan.bales — Fri, 27 Jul 2018 21:04:51 GMT

In the sweep settings there are options for orientation, perpendicular or parallel, as well as using guide rails instead of just one single path. Chances are we can get it to work.

You can share a public link and paste it in this thread or simply export the file and upload it here.

Re: Sweep Problem

ahmed_afathalla — Sat, 28 Jul 2018 06:56:50 GMT

Hello Ryan,

I did all sweep settings combination and nothing worked I'm sharing the design link below may be you could find a solution for that problem.

https://a360.co/2mRPtIV

Thank you,

Ahmed Fathalla

Re: Sweep Problem

davebYYPCU — Sat, 28 Jul 2018 08:52:55 GMT

Gooday Ahmed,

You were so close, when I reviewed the file, the sweep profile sketch had a missing projected (yellow) point,

The first error message was that the path was not connected to the profile.

Now lots of steps to fix the model, but fixing the sweep was the easy bit,

you will see changes to your sketches for that.

I cut off the tab next to the sweep profile sketch, to provide the path - top face edge.

Your sweep updated and worked immediately. Great, but did not try other sweep options.

Put the tab back on, (new body and sweep cut it with the same input. (To match the pointed end as it was drawn.)

Shaped the new body and combine joined it back on.

But as per photo, the path was not long enough to cut all the body, a small section not reached was left over.

You can check my timeline, for the fix to cut that out.

Might help,,,

File attached....

Re: Sweep Problem

ahmed_afathalla — Sat, 28 Jul 2018 23:40:48 GMT

Thank you Dave for the solution, I guess I was missing the tab next to the sweep, I have an extra questions if you don't mind:

1) How did you manage to add 2 profiles for the sweep, I could only add one at a time but your solution has 2 profiles added, how can I do that?

2) I know the first profile would be the small window to cut inside the frame slot what's the 2nd profile you are choosing.

2) How do you select the profile inside the frame, I mean how do you pint at it.

Thank you,

Ahmed

Re: Sweep Problem

davebYYPCU — Sun, 29 Jul 2018 04:31:17 GMT

Ok, I think I know what you’re asking.

I am away for a couple of hours yet, so it’s my opinion, without testing it.

1. Nope, 2 Sweeps, one (different) profile for each.

2. When I first got the Sweep to work, your original profile created a tunnel in the curved end,

similar to yours but almost right, so I made your profile wider to take the tunnel wall out, to the inside of the curve. (Wasn’t dimensioned)

At that time the the profile sketch was not divided, so having done that, Sweep, I had to return to original profile when Sweep cutting the tab, edit sketch and added a new dividing line at the old size, and so I selected the smaller side of the profile for the second sweep through the tab.

3. I hide the body/s during selection, prefer to see what I am doing, love the lightbulbs.

I don’t use selection filters, and I don’t often use the long left click either.

So it’s a quirk in Fusion (smarter than we are!)

if it is showing I selected 2 profiles now in the dialogue box, that isn’t how I built the model. Sketches have no history, but Fusion must have joined the two in the background, when you come back to inspect it, it knows I used the big profile first, then divided it.

My story and sticking to it.

Hope that helps...