It seems you are curretly editing Sketch2. If you are, this will take priority over whatever you select in the feature tree.
Try to exit sketch - THEN select Sketch1 and Revolve.
>>It seems you are curretly editing Sketch2.<<
Thomas -- You are right. Thanks.
That solved **both** problems, as the two solids now seem to have merged into one as they should. The only trick was to add a second centerline to the second sketch.
It appears that there are two choices about when to add this second centerline. Easiest may be to add it after the first revolve, when you can't see the first centerline. It also appears possible to add it directly to Sketch2 (which also shows the first centerline), ignoring the yellow box, as long as it's a different length from the first. Then it appears possible to distinguish between two co-linear centerlines when doing the second revolve. Any guidance on this subtlety? -- John Willett
Additionally, you could still create Sketch2 after the first revolve. All you would need to do is show Sketch1 and make all your references to that sketch instead of the solid geometry. I do this all the time.
>>All you would need to do is show Sketch1 and make all your references to that sketch instead of the solid geometry.<<
Roland -- I've been trying to do what you suggest (selecting Sketch1/perpendicular and filtering for sketches only), but whenever Sketch1 is visible inside the revolve and I try to draw the center-point arc, it gets added to Sketch1, not created as a separate sketch. The only way I seem to be able to get a new sketch is to not show Sketch1, but then I appear to be referencing edges of the first revolve, not points on the Sketch1, even with the filter set. What am I missing here? -- John Willett
Apparently you are only editing the first sketch and not actually starting a second sketch. Make sure you are clicking the right buttons/menus.
>>Apparently you are only editing the first sketch and not actually starting a second sketch. Make sure you are clicking the right buttons/menus.<<
Roland -- Can you please be more specific? I'm not getting anywhere with this! Everything I try either edits Sketch1 or references the solid model (now called Cylinder) instead of the Sketch1 (now called Rectangle) in the new Sketch2 (now called Center-PointArc).
Or maybe I'm interpreting it wrong? Below is a new screen shot of editing the Center-PointArc, showing the sketch relations:
Under the entities list for the start of the arc on the top right corner of the Rectangle sketch (also the corner of the Cylinder solid, of course!) it says that Point6 of the "same model" is coincident with Point1 of the "current sketch." I'm not sure exactly what this means, but I had expected to see some point in **Rectangel** being coincident with Point1 of the Center-PointArc.
Anyhow I can confirm that the Center-PointArc must not have referenced the original Rectangle sketch (marked "show" in the above screen shot so that its outline is visible): When I delete Cylinder without disturbing Rectangle, this causes dangling entities in Center-PointArc and failure of the Revolved Thin feature based on it. Note that this did **not** happen in the case above, when the two sketches were defined before either revolve.
In general, how do you tell whether a point in a new sketch is coincident with a point on a solid part or a point in the underlying sketch? -- John Willett
>>When I delete Cylinder without disturbing Rectangle, this causes dangling entities in Center-PointArc and failure of the Revolved Thin feature based on it.<<
OK, Guys -- I eventually stumbled on a way to fix this problem. Center-PointArc/Edit Sketch and more careful examination of the relations with Display/Delete Relations PropertyManager/Filter=Dangling for Relations=Coincident1/Entity=Point6 indicates "Entity=Silhouette Vertex of RevolveArcAfterCylinder." This is obviously part of the problem, but it is not easy to fix because I can't click on the corner of Rectangle that I want to replace it -- it's covered up by the point on Center-PointArc with the bad relation. The only way I've found is to replace this relation for Point1 with another (inappropriate) point on Rectangle, revealing the upper-right corner of Rectangle that I actually want. Then I replace the same relation again with that point, re-build Cylinder (yielding, incidentally) the identical result I got with the sketch-only method outlined earlier), and all is good.
This is a very involved and error-prone procedure, and requires correcting the other end of the arc (which moved for some unknown reason); but it actually does work. Is there no better way of repairing the problem after the fact?
Fundamentally, I still don't understand why filtering for sketches didn't allow me to select the correct point on Rectangle for the relation in the first place. There must be a correct way to do this after building Cylinder, but what is it??? -- John Willett
Actually filter "Sketches" PREVENTS you from selecting the point you want. It filters entire sketches only. You want to use Filter Sketch Points (just to the left of Filter Sketches) also to select line endpoints.
Another option for you is to right click on the point and use Select Other and select from the list.
>>Actually filter "Sketches" PREVENTS you from selecting the point you want. It filters entire sketches only. You want to use Filter Sketch Points (just to the left of Filter Sketches) also to select line endpoints.<<
Perfect! The combination of Sketch Points and Sketch Segments filters allowed me to set the two relations needed to points on Rectangle in spite of the presence of Cylinder.
>>Another option for you is to right click on the point and use Select Other and select from the list.<<
OK, I can see the list of choices after right-clicking the point in question, but there are problems:
1) [Maybe I was previously confusing the new (1) here with (2) below:] When trying to sketch Center-PointArc on the Cylinder solid with Rectangle "shown," right-click/select-other on either of the points that lie on both the cylinder edge/corner and the rectangle segment/corner does not produce a selection list. Should it?
2) [My original statement was incorrect. Fixed here:] When editing the Center-PointArc sketch **before** deleting Cylinder, choosing the point from the list that I think is correct (on Rectangle as opposed to on Silhouette or Cylinder) does not "take" unless I remember to go through the Display/Delete Relations process (detailed below) first. I suppose this should have been obvious, right?
3) On the other hand, replacing the dangling reference after deleting Cylinder and selecting "Stop and Repair" **does** correct the error, but only if I follow several non-obvious steps:
a) Show Rectangle -- This step appears to be critical for getting its points/segments onto the list in **either** case.
b) Choose to edit the Center-PointArc sketch.
c) Click Display/Delete Relations and select the problem relation (or filter for "Dangling")
d) Select the erratic point from the pair in the Entities list to "light up" the replacement box
e) Do your right-click/select other-trick on the point with the highlighted relation in the display window and select the correct point from the list
f) Click Replace in the Entities box and the green check in Display/Delete Relations PropertyManager
g) Rebuild the model.
Does this sound about right?
Going through these exercises, I finally noticed how to tell what sketch/solid a given point is referenced to (look at "Entity" listed in the "Entities" box in the Display/Delete Relations PropertyManager)!
I apologize for so many edits. This has all been a big help. If a second "Answer" were possible in a thread, your suggestion would deserve it! Just question (1) remains unless you have other comments on (2) and/or (3)... -- John Willett