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Sketcher - limiting constraint reference scope?

As applicable to dimensioning and constraining a section; is there an option to limit the scope of selectable entities to established References and Sketcher geometry?

I do not want the Dimension or Constraint to latch on to any (model) entity other than defined Reference entities and Sketcher created entities or watch the Pre Select light show as (would be) inelligible entities are highlighted.

The desired effect would be similar to a persistent Reference Entity selection filter.

My workaround is Hide all Layers, which include def_layer layer_solid_geom and layer_features. It's nice enough in its own right for the clean screen but thought I'd ask the question anyway.

Reply to
gluteous maximus equus
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There have been a bunch of partial solutions and none that really match what you're asking for. Only one new piece of functionality governs default reference selection. It's a config options called sketcher_auto_create_refs but this really only applies to getting into sketcher. As of WF3, you can get into sketcher without picking any references, then establishing references as you constrain and dimension. If prehighlighting is irritating, go to the Model Tree Settings menu and uncheck Prehighlighting. An old solution to the autodimensioning/constraining dilemma was to turn off Intent Manager. Other more reasonable methods of limiting references to only those that are desirable include some of the following:

  • Putting features like rounds and holes toward the end so that these don't become feature references
  • Using Insert Mode to place the sketch where only certain references are available
  • Picking features and RMB 'Hide' which is about what you're doing now but a little more direct, less global.

The solution might be for PTC programmers to write a program that dimensioned/constrained to references that I've already selected rather than an option called dont_be_stupid set to YES! Why should we have to tell the program NOT to be stupid.

David Janes

Reply to
Janes

Thank you, Dave. That's the conclusion I'd come to but wanted to make sure I hadn't overlooked something. Thanks for the additional suggestions, as well.

Reply to
gluteous maximus equus

Yeah, it's too bad they haven't extended the functionality of assembly reference control ('Tools>Assembly Settings>Reference Control') to sketcher references to geometry in part mode. The assembly reference control lets you set what models you can (and cannot) pick the references from; it can confine references to pub geoms or to skeleton model geometry; for what it does, it's great but it's limited to top down modelling within an assembly. There's nothing comparable that works in part mode, though it doesn't seem like it would be a terrible stretch to get it to work there.

David Janes

Reply to
Janes

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