topic Re: Fusion won't let me make two splines coincident in Fusion Design, Validate & Document Forum

Fusion won't let me make two splines coincident

paramax55 — Thu, 17 Feb 2022 21:57:03 GMT

I'm trying to make some splines on an arch. I specified the inside of the arch, made some loft sketches, then lofted to get the outside of the arch (it's not a simple offset). I made another sketch (I couldn't project the loft onto the original sketch because it was earlier in the timeline) and projected all of the curves and lines that I was going to need. Then I specified my splines using tangent and perpendicular constraints. I tried to trim the original parts of the outside arc that I wasn't going to need, and I couldn't grab it. So I zoomed all the way in and I saw that the two splines weren't touching. I tried to delete the tangent constraint and apply a coincident constraint, but Fusion says the constraint already exists. In the zoomed-in screenshot, you can clearly see that they are not. I can think of some ways around this, but they will certainly be hacks that require extra steps.

This second screenshot is zoomed further out and shows where I am working

Betreff: Fusion won't let me make two splines coincident

g-andresen — Thu, 17 Feb 2022 22:09:13 GMT

Hi,

where is a problem?

günther

Re: Fusion won't let me make two splines coincident

paramax55 — Thu, 17 Feb 2022 22:15:02 GMT

Hello. The problem is where you circled "Tangent." By the time I made the screenshot, I had already deleted the tangent constraint.

I did some further checking and it looks like a big part of my problem is that I can't edit projected lines??? If so, what's the point of being able to get the computer to do some of the work for you (a loft), then use projection to move it to your sketch? Isn't the point of projection to get earlier work into your new sketch so it all matches up?

Re: Fusion won't let me make two splines coincident

davebYYPCU — Thu, 17 Feb 2022 22:19:35 GMT

if you project geometry to a sketch, you did that as a workflow step, why would you do that if you don’t want to keep the result, and need to edit it?

You have the choice of project without associative link,

Might help...

Re: Fusion won't let me make two splines coincident

paramax55 — Thu, 17 Feb 2022 22:26:10 GMT

The reason is that I have two things that I want to do. 1) There is an inner arch. 2) There is a protrusion on that arch. The end product will look like you took an arch, then made a protrusion out of clay, and blended them together. The arch would be "buried" in the new part. I am going to be using some surfacing processes to get my final product, so I will be unstitching and cutting before it's all said and done. The outside curves are dependent on the first arch, but I will need to cut it at the point of intersection in order to get the surface patch to work right later.

Is "project without associative link" an option in the project dialog box?

Re: Fusion won't let me make two splines coincident

davebYYPCU — Fri, 18 Feb 2022 00:24:23 GMT

Yes it is a tick box in the Dialogue Box.

Re: Fusion won't let me make two splines coincident

etfrench — Fri, 18 Feb 2022 01:02:27 GMT

Zooming in is not a reliable way to determine whether or not geometry is coincident or tangent. This is a display issue. If the geometry shows a closed boundary, then you can consider it coincident (if there are also no white endpoints). Tangent should always show an icon.

Re: Fusion won't let me make two splines coincident

paramax55 — Fri, 18 Feb 2022 01:40:52 GMT

That is not necessarily true. I have recently started working with surfaces. You can try to stitch two surfaces together that won't stitch. If you zoom in, you will see the smallest gap. If you try to measure the gap, it will measure "0". Jason Lichtman did a webinar on this and it helped me out of a jam.

There is also more than one thread on splines exhibiting strange behavior and it's listed as a known bug in Fusion. A lot of times, I have gotten errors like this if I try to "math" things together rather than having Fusion "snap" them together.

Re: Fusion won't let me make two splines coincident

etfrench — Fri, 18 Feb 2022 01:51:52 GMT

I agree, that's why I said it's not a reliable test (in sketches).

Re: Fusion won't let me make two splines coincident

paramax55 — Fri, 18 Feb 2022 02:00:40 GMT

Once I broke the link, I was able to do what I needed. Thank you.

Re: Fusion won't let me make two splines coincident

jeff_strater — Fri, 18 Feb 2022 02:06:31 GMT

@paramax55 wrote:

That is not necessarily true. I have recently started working with surfaces. You can try to stitch two surfaces together that won't stitch. If you zoom in, you will see the smallest gap. If you try to measure the gap, it will measure "0". Jason Lichtman did a webinar on this and it helped me out of a jam.

There is also more than one thread on splines exhibiting strange behavior and it's listed as a known bug in Fusion. A lot of times, I have gotten errors like this if I try to "math" things together rather than having Fusion "snap" them together.

A couple of things here:

the surface gap could also be a graphics issue, not a geometry issue. Just like with the splines themselves, surfaces are displayed using an approximation with triangles. There can be gaps that exist in the graphics that are not there in the geometry.
Measure is not a reliable way to measure gaps. It always reports the closest distance between the selected. So, if any part of the two faces touch, the distance will be zero.