Best way to explore electric wire routing over a design ?

[Anonymous]

Hello,

I'm designing a battery made of 18650 cells.

The cells have now a fixed position and the frame and clamps holding those cells are now also determined.

Now I need to explore the electric wiring of the cells and this step follows 2 goals:

1°) Find the most optimized path for the wires, which depends on the available room left on my frame holding the cells

2°) Determine the total wire length needed to achieve this wiring

To do that, it would be nice to be able to explore the possible paths as I would do it in real life:

- start the cable at point A (a pole of the cell), and this starting point will remain fixed as I continue wiring

- extend the cable to location B and again fix that point and continue wiring

- etc.

I would need to make the wire follow the existing structure shape for some segments of this wire (like following the curves of the cells for example).

I would also need to be able to remove previous fixed point of the wire path, for example when I want to explore a different path. This also means the wire should straighten back if I remove a point before which the wire was constrained to follow the existing structure's shape.

I have looked at some tutorials about creating wires in fusion360 but I'm still not sure what tools I should use to achieve the wiring exploration as described above.

How would you do that ?

From the tutorials I have looked at it seems you need to "think the shape of your wire beforehand", while I would prefer to create a given length of cable in the first place and only then begin routing its path and fusion360 would make the wire bending in realtime according to the last fixed position I have set (and we could imagine a max bending radius parameter here), or also bend the wire automatically if I ask to follow the shape of existing structure, and unbend the wire if I decide to drag the wire away. Is it possible ?

[jeff_strater]

Unfortunately, this is not really possible in Fusion today.  The only tool that Fusion has for this kind of thing would be a 3D spline, but you would very much have to manually route your wires, then use the Pipe command to create a representation of the wire itself.

This is actually a fairly challenging and interesting design domain.  In a past life (a long time ago), I was involved in a wire harness design tool, but physical routing of wires in 3D space is a tough problem.  I suspect there are systems out there that do this, but I don't know what they are.

Jeff

[Beyondforce]

Hi @Anonymous,

I will start with the Spline tool to draw and figure out the wire path (it also works with 3D sketching). Then I will use the Pipe tool to make the wiring.

If you want, you can attach your model, and I will screencast my idea.

Cheers / Ben
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[Anonymous]

Hi,

Thank you for your answers.

I have just tried the spline & sweep method as I never experienced those tools before.

The good news is the spline can be edited (add/move points) after sweeping, which gives the opportunity to modify the shape of the wire.

The bads news:

- when editing the spline, the wire created along it (using sweep) is not updated in realtime. I can still do my work like that by "guesstimating" what the wire shape will become after editing the spline but that would of course help a lot if the sweep could be updated in realtime as I edit the spline.

- when I edit the spline, like moving a point, it modifies the shape of the whole spline and there seem to be no way to prevent that. I was hoping the "fix/unfix" constraint could do that but you cannot fix/unfix a segment only of the spline, you can only fix the whole spline, right ?

The latter issue is much more restrictive for what I have to do. The only workaround (at least with this spline-sweep method) seem to make the wire using several splines. I have not tried yet but that should create the "segments" I was referring to. Those segments could then be edited individually, without interfering with the shape of the previous segment(s).

I'm going to have a look at that now and will report if it does the job or not (I foresee it may be laborious to keep the segments aligned at the junctions points).

[Beyondforce]

So, let me show you what I meant:

Cheers / Ben
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[Anonymous]

Thanks for your video Beyondforce.

Indeed the pipe way makes the initial wire creation much easier than with sweep.

Now the spline editing is already what I was doing, exactly as you show in your video. And you face the same issue as I was pointing:

- the pipe is not updated realtime, you have to edit the spline 1st and then the pipe is updated according to your modification to the spline.

When I mentionned realtime I meant the pipe would update immediatly as you deform your spline. Without this you have to guesstimate the thickness of the wire if you want to follow any given existing surface.

- editing a point will change the shape of the nearby wire, even past other points on the spline. And you cannot "fix" a segment so it does not move at all while you edit the rest of the pipe/spline.

So you have to make your wire using several splines in a row, which will make that work very time consuming when you have 200 wires to route. Although I'm lucky as I'll be able to copy/paste some segments from one wire to another in my design. But idk if using several splines per wire will then still let me easily find the total wire length.

[Anonymous]

Another issue I'm just experiencing:

If I use the align tool to align the beginning of my pipe to a surface, or make a clean junction between 2 pipes segments, then the spline doesn't remain aligned with the pipe. I can still modify the pipe shape by modifying the spline but with the spline being at an offset place (and possibly different orientation too !), which makes the pipe modification much more laborious, if not impossible to figure out (when the spline orientation also differs).

Is there a way to prevent that ?

[Anonymous]

Some feedback as I continue experiencing:

I dropped the pipe method to fall back to the sweep method. The pipe method is too much restrictive in term of curvature radius, I got the "pipe will intersect itself" error almost all the time and it is a pain to avoid (and solve) as fusion360 informs about the error only after you apply your spline edition. At least this notification should be given in realtime, as you edit your spline point. This would already make things much less a hassle. But realtime update of the pipe (or sweep) would be even more user friendly, and instead throwing you this error fusion360 could just prevent you to move your spline point where it cannot compute the pipe/sweep.

Anyway the sweep method is much less restrictive. I had some "illegal surface" errors at the beginning but then all went flawlessly and I was able to get my virtual wire much much tighter against the existing parts.

See below the difference in achievable result, first picture is using pipe and I was not able to get close to my cell clamping part and neither to avoid the wire getting out the cell holding plate area.

Second picture is using sweep and I can stay well within the plate area, get the wire really close around the clamps, and then even follow the wavy path made by the cells.

[Anonymous]

New question:

I saw fusion360 is able to give the measurement of a spline, which is a very good thing for what I planned to do.

Now to get a cleaner wire wave path over the aligned cells of my project I tried to use another method that I already have used to design the clamping parts:

I start by sketching circles that are concentric with the cells and a bit wider (due to wire thickness).

Then I sketch a second row of circles, tangent to the first row of circles, to make the curve following the wavy gap between each other cells.

And finally I use the trim tool to remove any unwanted segments from those circles and only keep what will be the optimized path around the cells.

The result is shown below in the picture. When I double-clic the remaining segment it glows in light blue showing it is a continuous path.

The question is: is fusion360 able to tell me the length of this blue path ? (made of trimmed tangent circles)

I don't seem to manage to measure it using the measurement tool. If fusion can't tell me the length of that path then I'll have to approximate it using a spline. Not something that will prevent me doing what I want to do but that's some additionnal work which I find is wasted time, and it would be a bit sad to have to use such an "approximative" workaround when such a software is meant to let you design things very precisely.

[Beyondforce]

Regarding the Pipe, you should have just changed the thickness, then you wouldn't get the intersection errors.

Now, regarding the measurement of the trimmed tangent circles, make sure the lines are coincident to each other, get out of the Sketch environment, and then you should be able to measure the line as one pic.

[Anonymous]

I have just tried the measurement out of sketch mode but I still can't get it to work.

Even out of sketch mode when I hover this line the subparts are highlighted (the arcs making the line).

I think the lines are coincident as when they are not it does not highlight the whole line when you double-click (which happens to me often when playing with the tangent constraint and then trimming), but here the whole line gets highlighted.

But if I double-click it out of sketch mode fusion informs me this is a "multiple selection" (at the bottom right of the screen). And then if I press the "i" key to get the measurement tool fusion automatically changes the selection to only keep 1 arc.

I went back into sketch mode to verify the coincidence and when I tried to move a junction point between 2 arcs I saw 2 new arcs appearing. I realized (although I already suspected it) I'm mis-using the trim tool which doesn't delete segments but superpose them to nearby segments (the trim description in the tooltip wasn't very clear for me about what the tool really does).

So I fixed this, deleting those unwanted segments, but I'm still unable to measure the line out of sketch mode. The behaviour of the measurement tool remains the same as before.

Also I don't understand why when I select a junction point between 2 arcs fusion informs me about a multiple selection. But if I hold click on that point there is only a single point in the list that pops up. One point, and the 2 curves (circle arcs).

Idk if I'm just missing something to do to merge those arcs into a single curve ? If I move the point then the 2 curves are moving with it, so I don't understand what would be wrong.

[Beyondforce]

Then I guess the only way is Spline.
If you can't achieve your goal this way, then I guess, you'll have to look for another system, which has the capabilities that your are looking for.

Ben.

[patrickautosm]

I am awaiting for the Route Feature in fusion just like we had in Inventor. When it can be expected.

[jeff_strater]

TBH, I don't know what the "Route Feature" is in Inventor, but you might want to check out the new improved 3D sketching UI, which I think can help in this sort of routing problem:  improved 3D sketching 

[patrickautosm]

I have used the New Sketch UI , but that's not my concern about. My
Concern is with Modelling Flexible Components like hose pipes and
Electrical wires. In Fusion we can Easily model them in Static. But
Inventory has a Route Feature which allows us to model Flex Items with
Dynamic Positions. I am mentioning a link video from youtube as Reference.

https://youtu.be/oEAyfD2nAl0

[jeff_strater]

yeah, Fusion doesn't have anything like that for flexible hose/wire modeling.  Sorry, I did not realize that was your concern.

[patrickautosm]

Is it on the Roadmap of Fusion 360 development?

[jeff_strater]

not currently, no.

[mdwormanX3R4X]

Also looking for help with this. Pipe makes sense for round wires, but doesn't work at all for ribbon cables which often require folds. It does look like Inventor has this functionality: https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2019/ENU/Inve...

Solidworks does as well.

Any idea if this will find its way to F360? @jeff_strater 

[jeff_strater]

as of today, there are no plans for any sort of native ribbon cable support in Fusion, unfortunately.