can anybody help me to answer my questiones of use the edge tool?

[bzhang-2]

Dear All,

I am very happy to join in PTC community, could anybody help to answer my questions below? in sketcher, "use the edge" tool can not pick up/ select the outside projected edge of curved surface, how can i solve the problem? thanks for your help in advance.

[ptc-5044466]

could you please provide a image or a part file.

i do not think there is any issue with use edge option...it can surely pick outside curved edge.

[ptc-4890452]

Try hovering over the the edge you want projectet, then right click and then left click.

Sometimes I need to right click before left clicking to get the edge that I want.

[dgschaefer · Accepted solution]

Depending on the surface geometry, the silhouette surface may or may not be selected. Creo is pretty good about it, but some still can't be used.

You can, however, make a copy of the surface and use the trim tool to trim it back to the silhouette edge. You need to select the surface quilt and a plane first, then look for the silhouette button on the trim toolbar.

[bzhang-2]

Thank you for all of your responses, i think all methods is helpful. but i would like to say it will works on a simple curved surface, not works on a little complicated surface. kindly please download the Creo 1.0 part file i uploaded:https://www.box.com/s/i3kv06yw8h1meqhssbsr, i would like to trim the looped surface and by utilizing the silhouette edge when viewing from front plane. but the silhouette edge seems like a looped 3D curve, so the trimming with a plane would not works. what tool can be used? please let me know if you have any ideas. thanks for all of your help.

[TomD.inPDX]

I think you are trying to extract the silhouette curve which is not an edge. However, I can see many ways that you can make this work for you.

I would suggest making an extrude surface in profile and then intersecting the two surfaces. Not you have a feature you can project.

[TomD.inPDX]

This is a tip on how to find the tangent to the edge:

Solidify the imported quilt. In the sketch, project the seam in the middle of the straight legs. The normal direction of the solidify will help you find the center. from there you can draw a horizontal and place a datum point on the edge. You can do this anywhere you need to have a guide.

[bzhang-2]

Thank you Antonius, but i don't think it is effecient and even we can find the tangent point, it still can not create the silhouette edge on the looped surface.

[TomD.inPDX]

No it is not efficient; I never said it was. But I can certainly use this data to create the desired edge.

There is another tool that should help to get the exact edge perfectly. I have not worked with it enough to give a qualified tutorial but it is worth looking into.

How close do you need this projected edge to be? With the data I collect with the above method, I can easily sweep a few surfaces to get really close to the of the part. If I need exact, I would explore the "tangent surface" feature by extruding the "floor" and joining the import surface.

[TomD.inPDX]

Never mind. The simplest way (still a bit of work) is to work with DXF files from a drawing view.

With drawings, you -can- project a silhouette edge in a parametric sketch. You then import (get data) the DXF into a interim part file and use the data doctor to clean up the file. The projected edges create 4 perfect datum curves of the edge your looking for.

Again, not really a straight forward process, but I managed to wrestle out the desired accurate result in the attached step file.

[bzhang-2]

Dear Antonius, thank you for all your efforts. yes, they are feasible method.

after some research, i found that using the "silhouette edge tool" in Tooling/casting Application might be the best way to creat the edge, what do you think?

[TomD.inPDX]

If that is the optional extension, I don't have it. I only have the core Creo Parametric module.

But if it is core Creo, please post more information if you get the chance.

Either way, I'm glad you found a solution that works for you. I agree that Sketcher should be able to capture a slhouette edge. In all the years of working with Pro|E, it -still- isn't reliable about using a cylinder's silhouette edge as a reference.

Thanks for the challenge

[bzhang-2]

Sorry for the confusion, Yes, switch to the Mould application then use the silhouette edge tool can create the edge.

Thank you Antonius, you have always been helpful and give us so many ways to get the issue done.

[dgschaefer]

I wasn't able to get the file you uploaded before it expired and I'd like to take a look. I'm certain the trim tool with the silhouette option will give you the exact edge you need. It may not properly interpret it as an arc, but it will be the exact silhouette edge.

Can you re-post it or send it to my email address in my profile?

[bzhang-2]

Hi Mr Doug, sorry for the later reply, when you response at the beginning of the discussion, i am not able to try your suggestion. but now i find you are right, the trim tool exactly can do it and it is very straightforward. thank you for your help. it seems that i dont have to repost it. correct? appreciated your help.