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Pierce constraint in Pro/E and Creo?

David_M
Participant

Pierce constraint in Pro/E and Creo?

Do anyone know how to constrain part of a sketch to geometry which intersects the sketch plane?

I've got a video here of this being done in SolidWorks: http://www.solidworkstips.com/content/index.php/solidworks-tips/46-01-pierce-relation

Thanks


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11 REPLIES 11

Re: Pierce constraint in Pro/E and Creo?

Hello David

Here is short demo of Coincident Constraint

Video Link : 2062

Vladimir

Best Regards,
Vladimir Palffy

Re: Pierce constraint in Pro/E and Creo?

Hi Vladimir

Thanks for the response. That only seems to work with the end of a curve though. What I want to do is snap to the point where a curve intersects the sketch plane.

Thanks

Re: Pierce constraint in Pro/E and Creo?

Hello David

If you need move your sketch to intersect plane you can offset sweep profile with dimension or use Trim At.. functions (RMB)

profile.png

Vladimir

Best Regards,
Vladimir Palffy

Re: Pierce constraint in Pro/E and Creo?

Thanks, good tip.

If it was the edge of a solid or surface, rather than a curve, would it have to be converted to a curve with Copy, or is there another way?

Thanks again

Re: Pierce constraint in Pro/E and Creo?

Copy and paste is a good technique

Best Regards,
Vladimir Palffy

Re: Pierce constraint in Pro/E and Creo?

To assist with this, I've attached a part. The idea is to line up the circle with the line where it crosses that plane. Would the Intersect command be relevant here?

Thanks

Re: Pierce constraint in Pro/E and Creo?

Hi, I'm out of the office - I will write to answer next week.

Have a nice day.

Vladimir

Best Regards,
Vladimir Palffy

Re: Pierce constraint in Pro/E and Creo?

Hello

Here is my solutions:Move Sketch to other (new) Sketch Plane

Video Link : 2066

Vladimir

Best Regards,
Vladimir Palffy

Re: Pierce constraint in Pro/E and Creo?

David,

Not sure if this is what you are looking for, but I have attached a model I created in WF 5.0 where I created a spline sketch. I then invoked the sketch tool again this time while setting up the second sketch plane, I selected the point command and placed a point on the first spline curve, and on the datum plane (could be any surface though). After creating the point, I then selected the datum plane tool. I placed the Datum plane to go throughthat point, and to be normal to the original spline curve. After completing this plane, I allowed sketcher to use this for the sketch plane, and then created the circular sketch. It is pretty neat when I use Dynamic Edit, I can watch the second sketch stay tied to that intersection of the curve and plane, and also observe the curve remains normal to the spline at all times.

Hope this is helpful to someone.

-Greg

spline_int_plane.jpg

Re: Pierce constraint in Pro/E and Creo?

Hi Gregory

I did try a datum point like this and it does work very well, but I thought that there may be a way to do it in sketcher alone. If not, I think this is the way to go.

Thanks

Re: Pierce constraint in Pro/E and Creo?

Let me preface what I am about to say by saying I am currently on WF 5.0 so not sure about the work flow in Creo.

You can always create that point on the fly as you are creating your sketch as well. If you are already in sketcher mode, and then decide that you want to be able to reference the intersection between a curve/ edge/ axis etc, and a given surface; then activate the Datum point (not sketcher point) tool. after you have done this sketcher is placed on pause as you generate the point. While in this pause mode, select the curve/ edge/ axis etc. and the plane that defines the intersection, in this case, the sketching plane. After fully defining the point, take sketcher out of pause select the point as a reference and then you can use this point to constrain your geometry using coincident etc.

I have added a sketch to the previous model and given it a different name to clarify what I am referring to. Dynamic edit also looks cool with the spline here too, and you can watch the sketch move along with the intersection.

Hope this helps!

-Greg

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