Why this extruded cut error?

[Dave H]

Can someone tell me why the D-Profile cut throws an error?

First step was to sketch the circle needed for the OD of the piece.
Then extrude it.
Then sketch the D-Profile on an end surface.
Then extrude cut that.
Then sketch the small notch in the OD.
Then extrude cut that.
Then, suddenly, the D-Profile Cut is in italics.

It works, but I'd appreciate an explanation if anybody has one.

 

[DavidJ]

Did you possibly project to sketch using maintain association between the initial profile and the sketch for the D ?

If you did then changing the profile by adding the notch means the projected source entity is no longer available.

It would have worked fine if you had added the notch as a separate (3rd) feature, after the D.

 

[Dave H]

Did you possibly project to sketch using maintain association between the initial profile and the sketch for the D ?

If you did then changing the profile by adding the notch means the projected source entity is no longer available.

It would have worked fine if you had added the notch as a separate (3rd) feature, after the D.

Did not use "Project to sketch" at all.

So, modifying my first sketch by adding the notch after I added the "D" extruded cut results in the error? (I did not know the blank material had a notch until after the "D" cut was added)
But if I had added the notch as a separate feature, (rather than editing my first sketch) will not? :?
Or, if I had included the notch in my first sketch from the beginning, there would be no error?
Bizarre. Sometimes in the real world you have to go back and edit existing sketches. Shouldn't result in errors unless there is a problem with one of the sketches....

 

[DavidJ]

Did you dimension anything to the bottom of the original circular profile ? (which was cut away by your notch).

I notice that the D is 'position undefined', anything to do with D3,4,5,13 or 14 which are no longer used?

 

[Dave H]

Did you dimension anything to the bottom of the original circular profile ? (which was cut away by your notch).

I notice that the D is 'position undefined', anything to do with D3,4,5,13 or 14 which are no longer used?

The original D profile was drawn about the center of the OD (Origin). I may have added then removed a dimension to the bottom of the OD just to check my positioning. I will check on those if you can tell me where to find them.
I thought if a dimension was removed, it was "removed". Not leaving a trace.
Thanks David. I will investigate when time allows.

 

[albie0803]

I think what has happened is that you have drawn the D-Profile on the face rather than a plane.
From reading here I understand that entities like edges, faces and points get given internal reference ids which get modified when the entity get modified.
When you edited the face by putting the notch in, the face was given a new reference id which now no longer agrees with the original face id that the d-profile was constructed on (internally).
Helps to understand why we are told to put sketches on planes rather than directly on faces.

Hope that all makes sense.

 

[Dave H]

I went back through the sketches and found a centerline diameter around the perimeter of the original extrusion. How it got there is a mystery to me. Probably put there when I put in a check dimension, then deleted it. Anyway, once I cleaned that up the error disappeared.

 

[albie0803]

The perimeter circle is somehow related to your original extrusion. You changed the shape of the extrusion so the link ended up damaged, which was what the status error implied. Which is why deleting the line fixed the error.