How to mirror a sketch, and revolve it about a centerline EXTERNAL to the sketch?

[dlau-3]

Hi,

I'm using Creo 2.0 and trying to revolve a mirrored sketch using a centerline that is outside the sketch as the center of revolution (specifically, an axis datum I made by intersecting two planes). However, when inside the sketch, I used the "centerline" sketch tool in order to provide a line with which to mirror the sketch about. Because the sketch contains a centerline, the revolve feature automatically thinks that I want to use this internal sketch centerline to revolve the sketch about, but this is not allowed to happen because "All entities must be on the same side of the revolving axis." Thus, the section is deemed incomplete, and I cannot complete the sketch.

How do I tell Creo I want to use an external centerline, not the one I used in the sketch, as the axis of revolution?

Thanks for your help

[dschenken]

It's an option when you are creating the feature, but outside of sketcher. I always made it a habit to sketch a revolve centerline before anything else in a sketch due to long habit and don't know how to fix it if it won't let you leave sketcher to pick a revolution center. You can save the sketch and re-open it if you do have to quit.

Creo Parametric Help Center To Define an Axis of Revolution

[jzwijsen · Accepted solution]

When making the sketch add the external axis as sketch reference. Then create a revolve centerline and align it to the axis reference. The revolve feature will now use that revolve centerline instead of any other construction centerline in the sketch.

Regards, Jan

[jmonk1]

I always thought the feature was revolved around the first centreline you draw?

[Patriot_1776]

In the Olde Days, this was true, and it was a PITA.  Years ago they added the ability to pick any centerline, or use an external one.

[krowland]

There is a work around to what you want.Hit revolve and go to sketch, create your axis and sketch half the section without mirroring. When you click ok it will say not solid (just hit ok) and will revolve a surface around that axis. At this point, you can click in the box (top left) and choose the external axis for the revolution. Then go back into your drawing and mirror the sketch. Once you hit ok you will have to change the feature from surface to solid and hit the checkmark to finish. Long process but it will get what you asked.

[dlau-3]

This is definitely a possible work around. Thanks for the suggestion.

[Kevin]

The only way I've found to do this is to remove the mirror axis from the sketch temporarily so that it can be selected as the revolve sketch and the external axis can be selected as the revolve axis. You can then go back and redefine your sketch to add the mirror axis and specify the symmetric constraints and/or re-mirror the geometry.

[StephenW]

Based on your question, you made a sketch with a centerline in it.

You have an axis in your model.

You are making a revolve feature using the sketch (external to the feature) and you want to use the datum axis you created as the revolve centerline.

Create the revolve as you have been, when you have the sketch pre-selected or you select it in the feature, it assumes you want to use the centerline in the sketch (as you have discovered). Simple solution is to select the axis selection box (which by default says internal axis) and then select the axis you created. It will let you choose any axis to replace the internal centerline.

[Kevin]

If I've been able to recreate his problem, in Creo 2 M120 at least, the problem is Creo won't allow you to select the sketch if it has a geometry or construction centerline defined in the sketch. Creo also doesn't allow it to be pre-selected in my case. The sketch as I understood it is different than what you have shown, he used the centerline in the sketch to mirror geometry about it so he has a sketch with geometry symmetric about the internal centerline which causes the problem. This is what I understood to be the issue:

Sketch internal centerline removed to create revolve:

Centerline re-added to revolve and geometry re-mirrored:

[StephenW]

That makes sense then. The devil is in the details. A work-around is then necessary.

[jmonk1]

This works for me:

Gives me this:

Is that what you need?

[krowland]

jmonk - that will work but he was asking to use an external axis.

[jmonk1]

The first axis can be placed on the external axis if it is specified as a sketch reference. Have I missed something?

[krowland]

No, you are correct but in his message he stated that he physically wanted to pick the axis in the 3D model ("outside the sketch") and not reference it in the sketch. Your explanation is how I do it and is correct.

[dlau-3]

Yes, I think you guys are right. Looks like I HAVE to reference the external axis inside my sketch. Thanks for the help.

[dguillette-2]

in this case the axis of revolution has to be in the sketch.

it can be placed in the sketch at anytime...but...you have to define it as the axis of revolution.

select the desired center-line right click and select "designate axis of revolution" from the pop-out

[dlau-3]

Wow, first time user here, and I'm delighted by all the helpful people out there. Asked a question, left work, and came back the next morning with a ton of suggestions. I gave the correct answer to JAN ZWIJSEN because Jan was the first to suggest referencing the external axis in the sketch and using it as the axis of revolution before drawing my "mirror" centerline. Since it seems like there is no way to reference an external axis without first making an incomplete sketch, going out of the sketch, selecting the axis of revolution, and then going back into the sketch to complete it.

I really appreciate all the other and similar suggestions. Thanks for your help everyone! I learned there are a couple different ways to work around it.