Automatic Sketcher Reference Plane

[dgschaefer]

Creo2 M120

When creating a sketch, Creo will sometimes automatically select a reference plane.  Many times that isn't the plane I want to use, so I always go back and check it.

Is there a config option to force Creo to prompt me for a reference plane?  I searched the config editor and came up empty.


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[BobSchwerdlin]

Doug,

While in the process of creating your feature, but just prior to entering the sketcher environment, RMB and select, Define Internal Sketch. From there, you can select the sketch plane and the reference you would like to use from the pop-up "references" window on the right.

Bob Schwerdlin
Sr. Design Engineer
Dukane Corp.
2900 Dukane Dr.
St. Charles, IL 60174 USA
630-679-1941 direct
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www.dukane.com/us

[dgschaefer]

Thanks, I'm aware that there are ways to enter the sketch environment to ensure that I'm prompted for a reference plane.  Going to the placement tab and clicking "define" works as well.

However, the ability to directly select a plane and to be taken into the sketch environment is handy.  The problem is that a Creo isn't always good at orienting the sketch how I want or at choosing a reference plane that doesn't add new parent child relationships.

For those reasons I want to be prompted for that plane regardless of how I enter sketcher.  I had thought there was a config option for this.

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[BobSchwerdlin]

I saw a Creo 3.0 demo recently that showed some new options when entering the sketcher environment. The most important one I found was the ability to select a feature creation tool (i.e., extrude) and sketch immediately on any face, even ones that were oblique to ANY other surface, without having to first setup construction reference or planes. That could be handy at some point.

Bob

[bkurth]

I believe this is the config option you are looking for.

sketcher_auto_create_refs
0, 1, 2
0—Does not create the dimensioning references automatically.
1—Automatically adds orientation references as dimensioning references.
2—Automatically creates two dimensioning references.

Setting to 0 should force you to have to pick all your references, every time.

We are on Creo2 M090

Hope this helps...Brian

In Reply to Doug Schaefer:

Creo2 M120

When creating a sketch, Creo will sometimes automatically select a reference plane. Many times that isn't the plane I want to use, so I always go back and check it.

Is there a config option to force Creo to prompt me for a reference plane? I searched the config editor and came up empty.


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[dmartin]

Brian,

I believe that config option only affects sketcher references, not the orientation reference plane.

Doug,

I don't believe there is a way to force prompting for the orientation reference plane.

David R. Martin II

Senior Mechanical Design Engineer

Amazon

[mbrockman]

Doug,

It seems that functionality disappeared when they dropped wildfire. We used to be promped for the orientation reference / plane prior to entering the sketcher. I prefer to control the orientation. This "new" way eliminates 1 selection click. Was that PTC thought? I wonder if PTC could enable this "old" method for us old guys who like to discipline their sketches.

[mbrockman]

funny, that functionality exists when creating external sketches but not extrudes

[dgschaefer]

It depends on how you enter sketcher. If you select a plan and then pick sketch you go right into sketcher, Creo picks the ref plane.  If you pick sketch first, then you’re presented with the sketch setup dialog.

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