Hiding a sketch

sören_svensson

Hi,

Does anyone know how to hide a sketch so it doesn't show up on screen?

I create a sketch in FS and revolve it, but in the UI, both the revolved body and the sketch are visible.

I've tried the UIHint.ALWAYS_HIDDEN but no luck.

Regards
Soren

ilya_baran

Hi,

The ALWAYS_HIDDEN hint is for the parameters, not the geometry produced by the features.  You have two options.  If you never want to see the sketch,  within the feature, once you're done revolving the sketch, you can call

opDeleteBodies(context, id + "deleteBodies", { "entities" : qCreatedBy(id + "yourSketchId") });

The other option, if you want to hide the sketch temporarily is to just click the eye icon that appears next to your custom feature in the feature list when you hover over it.

Hope this helps.

ilya_baran

The answers to your questions are tied together.  When you delete a sketch from the feature list in the UI, you are removing it from the regeneration "recipe", as if it was never there.  But when you call opDeleteBodies, you are *adding* a new operation to the regeneration (in this case, inside your feature), after the sketch has already been used.  That's why it needs a new id -- because it's a new operation.  It's like the difference between removing the feature that creates a part and using the "Delete Part" feature (next to the Transform feature in the toolbar).

ilya_baran

Hi,

The ALWAYS_HIDDEN hint is for the parameters, not the geometry produced by the features.  You have two options.  If you never want to see the sketch,  within the feature, once you're done revolving the sketch, you can call

opDeleteBodies(context, id + "deleteBodies", { "entities" : qCreatedBy(id + "yourSketchId") });

The other option, if you want to hide the sketch temporarily is to just click the eye icon that appears next to your custom feature in the feature list when you hover over it.

Hope this helps.

cadmando

Click on the eye on the right side of the sketch you wish to hide in the Features List

sören_svensson

Thanks!

opDeleteBodies did the trick.

two things I don't get with that function

1) why does it need a new id (id + "deleteBodies")?

2) in the UI, if I delete a sketch, bodies based on it disappear too, but not here (from FS), how come?

Regards
Soren

ilya_baran

The answers to your questions are tied together.  When you delete a sketch from the feature list in the UI, you are removing it from the regeneration "recipe", as if it was never there.  But when you call opDeleteBodies, you are *adding* a new operation to the regeneration (in this case, inside your feature), after the sketch has already been used.  That's why it needs a new id -- because it's a new operation.  It's like the difference between removing the feature that creates a part and using the "Delete Part" feature (next to the Transform feature in the toolbar).

ber_ta

You can create a new context and create a sketch inside this context. I did it and the created entities are not shown in feature list nor in viewport. But it seems that you can use all operations on them. Query ... evalute ... at leaste these somes i used were no probleme.

Maybe this is what you was looking for.

Regards
Stephan

ilya_baran

@ber_ta
That won't work if you want to use the sketch for creating solid geometry in the context you actually care about -- if you make such a sketch, you have no way of making e.g. an extrusion based on it that you end up seeing (unless you merge the contexts, in which case you also get the sketch).