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Ronald11-Visitor
1-Visitor
February 27, 2013
Solved

How to avoid double intersection points.

  • February 27, 2013
  • 2 replies
  • 4216 views

Everybody,

I have a situation where i need a point at the intersection of a cycinder surface, with two datum planes witch are normal to each other.

This wil create two possible intersection points on the cylinder surface.

When I variate the cylinder diameter parameter, the intersection points sometimes switch from the left to the right & vica verca.

I noticed this because I had placed two datum points on the intersections (pnt1 & pnt2), and they switched position.

So my question: Is there a way to overconstrain this point ,or define a pos x-dim for this point, or define a quadrant for the location of this point,

so it always uses the intersection at the right side for example.

Ronald


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Best answer by TomD.inPDX

This "should not" be difficult at all. If I understand correctly, you want the point to be 5mm -outside- the angled line, right? The way the sketch is currently constrained, it has only one solution, right (bound by the coincident with the vertical line)? So make an analysis feature (simple measure length) of the construction line and dimension the "point" on that line with a relation of "Measure-5".

If I under stand correctly and the problem feature is the 5mm line, this should solve the problem of the short line flipping about the angled line.

Here is another trick that overcomes a serious problem with scaling sketches. The problem is making too big a jump from the previous version. You could, through relations, limit the amount a sketch is scaled by limiting the difference from step to step. Say you have a 1000mm dimension and changing this more than 100 at a time causes errors. You could force a relation to revert to the maximize the jump 100 only if the input is greater than this.

The only other problem I can see is that the sketch could flip the large angled line as well under some conditions. In this case too, you can place a dimension and have a relation test this condition to make sure the angle is within a range or some other construction geometry is within an expected range. If it fails, you can have it go to a default value or simply revert the change to the original value.

I know one shouldn't have to do this, but as one that has come to rely on sketches for some very stable scaling and evaluation, it -is- possible.

2 replies

C
Constantin15-Moonstone
15-Moonstone
February 27, 2013

You might try to create a copy of only one half of the element (cylindrical surface or edge) as a reference for the point.

Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
February 27, 2013

Best way, from what I THINK you want, is use a datum point offset from a cylindrical coord sys, and use relations to make the radius of the point the same as the radius of the cylinder.

Also, you can copy the indivitual 1/2 surfaces, and them merge them into one surface, and try that. I think the above method is more robust.

I've said this for over 15 years: I think a TON, if not most, of geometry failures is Pro/E cutting cylinders in half like that.

T
TomD.inPDX17-Peridot
17-Peridot
February 27, 2013

True that, Frank!

Ronald, there are many ways to accomplish this. My thought is to create a sketch with a line that is constrained to the cylinder on one end. Now place your point at the end of that line. The sketch will always update to the cylinder diameter.

It seems the concesus is that you don't want to use a feature that has two possible solutions.

J
Jeroen1-Visitor
1-Visitor
February 28, 2013

I'm working with Ronald on this, and I would like to add some more information.

If it was only for a cylinder, I agree there are easier solutions. But by changing parameters this cylinder surface can change into a cone or an eccentric cone, in both directions. And the point that we need is somewhere on the surface, not on an edge. In short, it's not that easy to define a sketch, we would have to calculate the local diameter to search for our point.

Our (short) experience with Creo is that trying to limit the possibilities of a sketch or surface by cutting parts of the surface or line, is not the ideal solution. Creo still knows the definition of the line, and sometimes it tries to extend the surface/line to search an intersection.

For static drawings, most things run smoothly. But when working with parameters, relations and pro/program to create dynamic parts, things go south now and then...

For another problem like this, I searched for a mathematical approach to calculate a value, in stead of doing it with a sketch. The sketch was very easy, the math wasn't. I also found out why the sketch failed sometimes...

While solving the mathematical equation, I ended with a quadratic equation, meaning that there are 2 possible solutions. One was the correct one, the other always gives a ridiculous low value (-60000 and lower).

By using math, it's easy to ignore the wrong value.

In a sketch it is not possible to avoid this issue.

Maybe it would be interesting that PTC would allow us to 'overconstrain' a sketch, or to define a range a dimension can have.

I think I have to search for another mathematical solution for this issue, unless somebody knows a way to add extra constraints in a skech.

If you want, I can post an example of such a sketch that can go wrong.

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