best way to model pinball ramp?

[shastada]

Hello everyone.  Been migrating from Onshape to Fusion360 lately, CAD novice (I'm a software engineer) so this might be obvious but I've been fighting fusion for some hours now on how to model a pinball ramp for a hobby pinball machine I'm making.  Here's a video of the foam core mockup I'm trying to convert:

  It's kind of like a lot of tutorials but different in some key ways.  Ways I've tried to tackle this:

1) Modeling the surface that the ramp sits on top of, then extrude/intersect the 2d top view of this on to it..

-> Patch I can't figure out how to mingle the 2 different paths

-> Model - I don't feel i have enough control to make a dimensionally accuate part

2) 3D sketch to come up with paths, and then sweep.

-> 3D sketch part is "ok"

-> Sweeping one of the paths goes ok, but trying to trim out the stuff I don't want is proving difficult.. Part of this might be the Boolean operands are acting different than i'm used to for onshape.

Here's a screencast in case I'm pretty close: 

http://autode.sk/2zZ1Wir

So, looking for advice on how others would approach it right now to see if I'm even tackling it the right way? or if you think there's some tutorials i'm missing if i'm even asking this question, by all means, set me straight! 🙂   I just don't want to do something super labor intensive as I will probably 3d print / iterate several times before I get it just right so want something that's robust to change.

[HughesTooling]

This thread might help.

https://forums.autodesk.com/t5/fusion-360-design-validate/puzzled-how-to-perpendicular-slice-a-curve...

Mark

[davebYYPCU · Accepted solution]

If you adjust and fillet the second path, onto the original, then you will be able to run the inverse sweep as a cutter, the sharp path intersection is the causing trouble.

Might help...

[mroek]

As @davebYYPCU says, using a cutting profile is often a good way to solve issues like this. Start as you did, and allow the two sweeps to join into one body. Then create a cutting profile (just add one line to your profile sketch to close the inside), and repeat the two sweeps (as cuts) with just the inside profile selected to remove the unwanted bits.

[Beyondforce]

Hey @shastada,

It will be great if you could share the file. It's much easier than you think.

Cheers / Ben
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[shastada]

Thanks for all the suggestions.  Back to the grindstone now / vacation over so not sure how quickly I will get to try them out.

[shastada]

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@HughesTooling wrote:

This thread might help.

https://forums.autodesk.com/t5/fusion-360-design-validate/puzzled-how-to-perpendicular-slice-a-curve...

Mark

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That's definitely a different approach!  Given I have two different slopes at the "fork' it looks like i'd need to do double the amount of steps overall, but I can see how it'll work.  There is definitely a different situation where I will use this!  As there's other replies where people think the sweep solution is "close" I will start with that.  But thanks! 

This is similar to this tutorial, no?

https://www.youtube.com/watch?v=hicToIPxYJI

[shastada]

here's the file attached, and a link. whatever is preferred

http://a360.co/2C9iGoP

I think i get the gist of the cutter now, will try that when i get a chance.

I'd be interested in any feedback on the 3d sketch itself.  I used points on various key height off set planes and drew the sketch through that.  The end result seems to be that I can't play with the spline too much other than by going to the individual points.  If there's a better way, (or , don't do 3d sketches in the first place) I'm all ears on that as well.

[shastada]

Ok spend the last week going back and forth between the two types of approaches:

1) Sweeps

- The inverse cutters did clean things up immediately, however what I was fighting after that was getting the sweeps to not twist such that the 2 exits weren't horizontal anymore.  Was trying everything and the tool kept throwing errors.  Tried the 'twist' field of sweep .. nope shape would just disappear and an error.  Tried guide rails.. nope, "Not smooth".  tried guide surfaces, also "not smooth".  Finally I kind of started over with a new 3D sketch of the profile.  Not doing anything specifically different but, for one, figuring out that if you want to adjust the curvature/tangent handles on a 3D sketch that is also a move/copy operation (can't just grab them) just like moving the points themselves.. that was kind of a breakthrough 😉    At the end I must of made it tangential enough that the 'twist' field of the sweep would take numbers without complaint and was able to ensure all 3 entrance/exits were horizontal.

2) Thicken surface

I spent most of the time trying to make this work.. since, the benefit of the surface thickening operation is that it's always going to be horizontal.  However that seemed to end where this approach did well.  I would end up with two sloping lumps that then trying to clean up (add side walls, remove the underside material, get the fork to slope into each other in a continuous way) was hurdle after hurdle.. I finally got something but it was 40 steps and felt super brittle.   After talking with a Mech E friend he steered me back towards trying to get the sweep to work, which after kind of rebooting was able to make that work

Attached where I ended up, now it's printing and figuring out adjustments and braketry