topic Center a point on a face adaptively in Inventor Forum

Center a point on a face adaptively

mmatanlevi — Mon, 19 Feb 2024 08:25:55 GMT

Hey. Let's say I have an extruded rectangle. Now I add new sketch on one of its faces and sketch a point. This point will be used as a location for a hole, for example. I want this point to be centered on the face even if the rectangle's dimensions are changed. Or, I want this point to be at the middle of one of its edges (Image attached, showing that I want the point to always be in same distance from left and from right).

If this is a simple case, I would like to complicate it with a case which I want to sketch this point of one of a metal sheet flange (image attached).

Thank you very much!

Re: Center a point on a face adaptively

YannickEnrico — Mon, 19 Feb 2024 08:33:09 GMT

Take a look at the constraint panel

Otherwise you can use a driven dimension and reference the other dimension to that

Re: Center a point on a face adaptively

mmatanlevi — Mon, 19 Feb 2024 09:14:52 GMT

Thank you very much!

For the first suggestion, Im sorry if its logically easy, but I dont manage to figure out how you keep it centered (or in a middle of one edge) by horizontal or vertical constraints.

For the second suggestion, I didnt know about that and after playing with that now I can see how it can help, nice.

Re: Center a point on a face adaptively

YannickEnrico — Mon, 19 Feb 2024 09:23:34 GMT

Simply choose one of the two constraints I highlit and choose the middle point of a projected line.

Horizontal/vertical constraint can constrain of of two things
A: A line to be either horizontal or vertical - Select one piece of geometry
B: A point to be horizontal or vertical in reference to another point - Select two pieces of geometry (center points of circles, points, end points, middle points)

If you hover, a dotted faint line will show you the direction it constrains. It's orange in my colour scheme. might be different in yours.

If you hold shift while using horizontal constraint, it'll constrain vertical instead, and the other way around.

Re: Center a point on a face adaptively

YannickEnrico — Mon, 19 Feb 2024 09:24:35 GMT

Middle point is easily constrained to. It'll show up as a green dot when you find it.

Re: Center a point on a face adaptively

SBix26 — Mon, 19 Feb 2024 16:21:44 GMT

Here is a sketch using Two Point Center Rectangle. Note that this tool automatically places diagonal construction lines so that the rectangle remains constrained symmetric around its center. You can use the same technique to constrain a center point on an existing rectangular face (only need one diagonal line, of course).

I use construction geometry and mid-points extensively when sketching to constrain things to be symmetric. I find them easier to comprehend than Symmetry, Horizontal, Vertical, and Colinear constraints, simply because they're visible.

Sam B

Inventor Pro 2024.2 | Windows 11 Home 22H2

Re: Center a point on a face adaptively

johnsonshiue — Tue, 20 Feb 2024 22:59:47 GMT

Hi! I could be wrong but I don't think this will work. To allow sketch geometry to solve adaptively, it is better to have as few constraints as possible. In this case, the center rectangle can be driven by multiple sketch lines and points, which may run into conflict of sketch solve.

Many thanks!

Re: Center a point on a face adaptively

JDMather — Wed, 21 Feb 2024 13:23:45 GMT

@mmatanlevi

Can you Attach your completed part?

I have another idea that has not been mentioned here - I would like to see if it will work with your Design Intent.

Re: Center a point on a face adaptively

kacper.suchomski — Wed, 21 Feb 2024 15:16:10 GMT

You can also create a construction point in a loop variant.

(view in My Videos)

Re: Center a point on a face adaptively

matthew.hansche — Wed, 21 Feb 2024 15:36:16 GMT

One thing you can try is using user-defined parameters if you are familiar with how they work.

I work with sheet metal extensively and I will occasionally create custom parameters which pull some of my other parameters (bend radius, plate thickness, flange distances, etc.) and create an equation such that the custom dimension will change to show a desired value as I change those parameters. Then, I will constrain the feature (a hole point, for example) but as the dimension I will set it to be the user parameter. Thus, that dimension will adjust as you change other features thanks to the equation you set up in your user-defined parameter.

I hope this is not too confusing...