Sketch Constraint to loop

[Christopher_Cardwell]

I have looked everywhere and haven't found anything close to what I need. I'm afraid it may not be possible. But let's give it a shot anyways. I need to create a sketch with a loop. We will start with an open loop for ease of use. I need to put a point coincident to that loop. The point will be moved based off a horizontal dimension. I need that point to stay coincident to the loop, and not a single line segment, as that dimension is adjusted. Here is an example of all the different segments that the point would need to travel on as it's adjusted. I feel like I have a clunky workaround if no one can come up with anything. But I really don't like it and I really don't like workarounds. Any help would be greatly appreciated. This is turning into one of those job altering projects that can take days and skill off of making new parts. This is the foundation of making that happen.

[CCarreiras]

Hi!

Have you thought about using a spline instead of multilines?

You can only constrain the point to one of the line of the multiline, but you can constraints the point to all Path of the spline.

[Sergio.D.Suárez]

Let's see if I understand you correctly, you have a horizontal parameter, let's imagine it is called X, as you advance a sketchpoint will move coinciding with the polyline you need. There is a solution based on mathematical concepts. You need to work with f(x)1, f(x)2, f(x)3 and transfer this data to ilogic to control the position of the point with 2 coordinates, X, and Y. for example: When X varies from - 5 to 5, Y will be located at f(x)1, a linear function with pending m1, when X varies from 5 to 15, Y will be located at f(x)2, a linear function with pending m2. and so on, I know it may seem complicated but it is a viable solution from a mathematical approach.
I imagine other ingenious solutions, for example creating a surface body with the lines you need and then creating an assembly with the surface part and another part that contains a workpoint. Using a suitable surface sliding constraint it may be possible to move the point with another constraint. If this works you could derive the assembly into a part file and get a result. I lean toward the first solution because it is something I handle frequently.

[Christopher_Cardwell]

I hadn’t considered that option really. The sketch will have to change angles based on inputs and there will be interior, intersecting lines that the spline will need to be parallel to in places. Basically offset from them. I’ve always been trained to stay away from splines so I don’t have much experience with them. If I can achieve these aspects for updating the geometry I’m good with going this route.

[Christopher_Cardwell]

When I get home I’ll post a true pic of the concept of what I’m doing. I think that’ll make things easier for me to explain. You may be on to something. I’ll just have to grasp how to apply it.

[JDMather]

@Christopher_Cardwell 

What version of Inventor are you using?

Can you Attach your *.ipt file here.

[Christopher_Cardwell]

Attached is the example file. This outline will be parametric and adjust based on input parameters. The two points that I placed in the sketch will need to move back and forth up and down the outermost profile. I can then get the exterior spreads based on the location of the exterior points. Hopefully this clears it up some. I am using Inventor Pro 2023. I am also attaching this file if anyone wants to look at it.

[kacper.suchomski]

Hi

This can be done in the assembly file, using translation constraint.

[Sergio.D.Suárez]

Here I share a descriptive video, and a file in Inv 2021. The method is applied for any type of function, in order not to complicate the introduction, use only linear functions (in many general cases of ilogic we work with constant functions, which are simpler still ).
There is something important in this approach. I have placed a dimension d7 to prevent the value of X from going through 0. In inventor we must prevent a dynamic parameter (a variable X) from passing through the value 0, because it runs the risk of making a "Flip" in the dimension, and turning dimension X to the left, this because inventor considers both dimensions as positive.