Sahaj Panchal's Blog

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Get correct ratio coupling in CATIA V5

Multi-sections solid (even multi-sections surface) tool is a little bit tricky for uneven sketches.

To apply the correct coupling for uneven shapes, say a circle and a rectangle, is a little tedious as you need to create same number of points on circle as the rectangle. And even sometimes you may not get the perfect matching points by manually placing them. So here is the solution to get over with. It may be a little lengthy but gives you the perfect result.

We are going to do so in a solid having two different end cross-sections, a circle and a rectangle with it’s corners filleted. So simply, start a new part file in Part Design workbench, you can name it anything for now, say Practice, create a rectangle as shown in the image below. Make it origin centric.


Apply fillets to the corners having 20mm radius.


Exit from the sketch and create a reference plane at an offset of 250mm from the YZ plane, side doesn’t matter. Draw a circle in a sketch on this plane having 100mm dia.

Now comes the ‘tip part’. If you try to create a multi-sections solid using these two sketches, in any coupling method, you may not get the desired result. So in order to obtain what you want, edit the second sketch(circle) and create a line (construction element) in any orientation.


Now, apply coincidence constraint to the end-point of this line with any two diagonal points of the rectangle. Consult the image.


And then create a point (standard element) at intersection of the circle and the line.


That’s it! Now use this point as a closing point on circle. So while creating multi-sections solid, right-click on the default closing point and select replace, and use this point.

This is what you will get. (make sure to select ratio in the coupling tab)


If you observe, still the sections are not coupled correctly. So what now? Well, do the same procedure for the remaining points! This is what you’ll do…


And then, while creating the solid, connect each point by defining coupling between them. As now in this case, each point of the rectangle is correctly coupled, you don’t need to switch the coupling mode to ratio.


Well, that’s it! This is a bit lengthy, but surely gives you the correct coupling.

What if the two sketches are not on the same plane? Say one is on ZX plane, and the other is on XY plane.


The procedure is same, including an additional step, in which you need to copy the rectangle in the second sketch. Make sure to convert everything, except the circle, to construction element, and create points at the intersection.


And in solid creation dialog box, apply the connect matching points as needed.


Even you can select supports to assign tangency or curvature continuity, and other required options of guide curves, spine etc. Obviously, you can apply this procedure to any number of sections. So the method is a bit lengthy, but it works!

That’s it for now! Come back soon for more!!Smile


One response to “Get correct ratio coupling in CATIA V5

  1. Raj Mishra July 21, 2012 at 1:39 PM

    Hi Sahaj,

    i was going through this post, Nice post. There is a better time saving option if you create points on circle using point on curve option and take length value zero reference points of rectangle vertex. You will directly get the points which you are creating using by creating line n taking intersection.

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