Constraining to a mulit-curve centerline

[Anonymous]

Hello,

I'm new to the forum and this is my first post.  I've been using Inventor for about 4 years now. I'll start with a bit of background related to my question:  I design pipeline inspection tools.  These consist of 2 solid bodies that are connected with a universal joint at each end and a tow bar in between.  The UJs can only deflect 71° before they jam and become rigid.  Certain pipelines have back to back bends and part of my job is to figure out whether our tool can navigate the S-curve without maxing out the angle on the UJ.  

I've set up a sketch with user parameters for variables like pipe diameter, wall thickness, bend radius, bend degree and the length of straight section between the bends (true back to back would be zero inches).  I've also got parameters for all the dimensions of the tool: body lengths, UJ tow bar lengths and the ride points on the centerline of the bodies which we best expect will follow the centerline axis of the pipe through the bends. 

 My problem arises when I try to constrain the ride points to the centerline of the pipe.  It will only pick up on the individual line segments and as I push the tool through the S-curve, I have to constantly unconstrain and reconstrain as it falls off the path, which is a huge pain in the butt.  I've tried to convert the curve to a polyline but it appears that it's only available in AutoCAD.  Do I need to make this curve some sort of spline?  I still need to tightly control all the parameters as I literally have dozens of these configurations of varying tools sizes and curves to figure out.  I thought maybe an equation curve would help but the math is a little beyond me at this point. 

I've also tried to do this in a 3D environment and just used a single body to constrain,  but I run into the same problem; Inventor does not recognize the centerline as one continuous curve.  

My only thoughts on a work around at this point is to extrude a small sweep surface with the top face following the centerline, and then extrude some small pins coming out from the ride points on the tool (where the dimensioning arrows are pointing) and doing a transitional constraint to have it follow the surface, but that seems like a huge pain in the butt considering how many tools I have to do.

Furthermore, eventually I'll need to navigate back to back bends off plane to one another, so getting a solid 3D solution to this would be fantastic.  Sorry for the novel,  I just wanted to give as much clarity as possible.  Thanks in advance for any suggestions.  cheers. 

[TheCADWhisperer]

What version of Inventor do you have?

Can you attach the files here that are shown in you images?

[Anonymous]

Unfortunately, I'm not permitted to export files.  I work for a giant mega-corporation and they'll spank me, I'm sure. 

[TheCADWhisperer]

I could easily create the wireframe sketch you show in your first image to show an example of Dynamic Simulation.

I recommend that you purchase the book by Wasim Younis.

You didn't answer my question of what version of Inventor you are using.

[Anonymous]

Inventor Professional 2016

[Anonymous]

I'd be happy to help if you could simply export the parts, but the answer is never consistent with each case. I also doubt that your company would spank you for exporting your files, they could be sued for that.

Best of luck to you and your inventor dreams,

Alvin

[Curtis_Waguespack]

Hi john.fraserKSPUV,

Using a spline for the sketch version might be all you need, depending on the end goal. Attached is a quick example file done in Inventor 2015.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Curtis_Waguespack]

Hi john.fraserKSPUV,

I goofed off with this a bit more just for fun and set up an ilogic form to (crudely) drive the sketch block. See attached.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[DRoam]

@Anonymous, have you looked into Transitional Constraints? I'm wondering if you could extrude your centerline path as a Surface and then constrain some geometry on your two cars to this surface with a transitional constraint. I'm not very familiar with Transitional Constraints and the intricacies of when they do and don't work, but I think this might be a good application for them.

[DRoam]

@Anonymous, this Screencast demonstrates something I think pretty close to what you're after, using transitional constraints like I described. The trick is to offset the "pegs" (which represent where your axles ride along the path) so that their inside face is centered with the car, and then use those pegs for the transitional constraint.

I would upload the files but they're in 2017 so they wouldn't do you much good. But if this looks plausible and you have any questions about it feel free to ask.

But it's fairly straightforward. Extrude your path as a surface, create a couple pegs on each car for the transitional constraint, then constrain your cars together like normal, then constrain them to the path with a transitional constraint (Constraint --> Transitional, pick your moving part [peg] first, then your guide surface). The only tricky part is making sure your cars are oriented properly before creating the transitional constraint.

Also, you'll want to create an angular constraint between your cars with limits equal to those your real-life device has. Then, if you car gets stuck trying to round a curve, you'll know it'll get stuck in real life. You might restrict the motion a little more than in real life just to be safe, so you can be confident that if the Inventor model makes it, your real-life device will.

[DRoam]

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@Anonymous wrote:

My only thoughts on a work around at this point is to extrude a small sweep surface with the top face following the centerline, and then extrude some small pins coming out from the ride points on the tool (where the dimensioning arrows are pointing) and doing a transitional constraint to have it follow the surface, but that seems like a huge pain in the butt considering how many tools I have to do.

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Lol, I just read this part... my bad  it's not really a pain in the butt though, it's fairly straightforward... unless you do have a bunch of different configurations, and then it could become cumbersome. Maybe building a single parametric model, and then building an Excel spreadsheet that you can use to drive your different configurations with iLogic and test them?

That's all I got... sorry for suggesting exactly what you'd already thought of 

[Anonymous]

Yeah, I've been messing with it a bit this afternoon.  I can get it to work as you did.  I thought for sure there would be a way to make it one continuous line in sketch mode, but I guess not.  Messing with splines was not giving me the parametric control I needed and kept giving G7 curves.  But I still was hoping to take it a step further and have it follow a back to back bend off plane. Seems awful silly that you can't use two "point" work features and constrain to a variable changing axis. If it was spline driven, I bet it would work although I'm not sure if there's even such a thing as a 3D spline.

[Anonymous]

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 "Maybe building a single parametric model, and then building an Excel spreadsheet that you can use to drive your different configurations with iLogic and test them?"

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Can I do this in the context of a single assembly?  Or would I need to adjust parameters for each body, the UJ and the curve in their respective part files separately?  I'm not all that familiar with using Excel to drive parameters. 

[kgilham]

This idea has been brought up a couple times.  We have an ideastation post that is trying to get more support.  https://forums.autodesk.com/t5/inventor-ideas/new-point-on-curve-edge-constraint/idi-p/3777983  Please go and give it kudos to let the Inventor team know that you would like this functionality added to Inventor.  The more Kudos it gets the higher priority it becomes in our backlog.

Thanks,

[DRoam]

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@Anonymous wrote:

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 "Maybe building a single parametric model, and then building an Excel spreadsheet that you can use to drive your different configurations with iLogic and test them?"

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Can I do this in the context of a single assembly?  Or would I need to adjust parameters for each body, the UJ and the curve in their respective part files separately?  I'm not all that familiar with using Excel to drive parameters. 

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I would probably build everything (the bodies, UJ, and the curve surface) as a multibody Part so you can control all the parameters in a single Part file. You can also program the max deflection angle of the UJ into this multibody file as a User Parameter, even though you won't use it at the part level.

Then push the two bodies and the UJ out into an assembly, constrain them, and in Parameters, Link in your multibody Part and pull in the deflection angle parameter. Then place an instance of your multibody and use the extruded surface path directly from the original multibody file for your transitional constraint.

This way all of your parameters are driven from the multibody Part, so you can build a Spreadsheet with all your configurations, have a text User Parameter in your multibody into which you type the Configuration name (you could make it a multi-value list if you have a known, fairly static list of common configurations), and when you chose the configuration, the iLogic goes to the Excel table and plugs in the correct value for each parameter. 

I wish you could use iParts for this..... but iParts are just so messy in Inventor and it would probably be even more of a pain in the butt isolating your bodies as separate members, pushing them out with the correct work geometry, pushing your path surface into its own iPart member, accessing that work geometry at the assembly level, etc. etc. etc.....

You might try iParts first (with just a couple, simple test configurations programmed into the table) and see if they'll work... but I doubt it, especially with your surface path, since iPart members don't seem to like including surface bodies in themselves, and you can't place the master iPart factory file itself.

The suggestion @kgilham pointed out looks great. You wouldn't have to create the pegs for the transitional constraint. However.... you would still have to move everything up to the assembly level. We would need a similar sketch-level curve constraint for you to be able to just check all your configurations at the part/sketch level.

[skylinejeff]

The idea center shows the idea of a path constraint as"accepted".

Any idea of a timeline to implementation? Would be very useful for us as well.