Rather then going through all the configuration one by one. It's simple enough to suppress a sketch in all configurations.
Any thoughts or tips?
Short answer is yes, you can suppress a sketch in all or selective configurations. Just RMB on the sketch and choose Configure Feature. From there you can easily select which configurations it needs to be suppressed/unsuppressed.
However, suppressing a sketch also suppresses any feature dependent on it. Suppressing will hide a sketch, but your post mentions hiding in the title and suppressing in the body. These are NOT the same thing. A sketch should exist because it is needed to define a feature. Hiding an unsuppressed sketch happens by default. Unhiding or showing a sketch requires an overt act.
I just did a simple test on a part with two configurations. I made a feature's sketch visible. Checking both configurations it was visible in both. Hiding it in one configuration did not hide it in the other. I agree there should be a way to hide/show a sketch for selective configurations just as you can configure the suppression state. Perhaps you can put this in as an Enhancement Request.
Linking display states to your configurations should create one display state for each configuration,
vice versa, if you unlink the display states, when you hide the sketch, it should be hidden in all configs until you change to another display state.
Go to your Configurations tab, right-click on a display state name at bottom, choose "Properties", and de-select "Link display states to configurations". That will create a display state for each configuration, but showing (or hiding) a sketch in one will show or hide it in all of them. Please don't ask me to explain why it works this way, because I don't know either.
Oh. Didn't have solidworks in front of me. :). I thought i was right.
Were you driving, Dan?
Dennis Dohogne wrote: Were you driving, Dan?
Dennis Dohogne wrote:
lol - My Mother always said "Nothing Said means Yes"
No, LOL. But thanks for the accountability!
I was at home with only my cell phone with me.
this does look like the best solution.
but its still shown in other display states. I guess you could toggle the option then set one display state to how you want the sketches or whatever to show/not show then deleted all other display states. you can then re toggle the link display state to config to create new display states for each config (if you need/want)
Alex Sully wrote: but its still shown in other display states. I guess you could toggle the option then set one display state to how you want the sketches or whatever to show/not show then deleted all other display states. you can then re toggle the link display state to config to create new display states for each config (if you need/want)
Alex Sully wrote:
A macro can be made to hide selected sketch in all configs OR may be selective configs.
From your question and heading I'm bit confused what you want to do i.e., hide the sketches of suppress the sketches ?
If you want to hide all the sketches from all configuration then see my attached photo. And if you want to suppress the sketches from all configuration then you need to make a macro or go into all configuration individually and suppress the sketch. But let me tell you that you only need to suppress the sketches for one time only. Then every time you open the part those sketches are suppress.
I'm asking if the functionality that is available to suppress a sketch in all configurations is also available to hide a sketch in all configurations. the solution you provide doesn't actually hide the sketch it just prevents one from seeing all sketches on the display. the sketches would still be set to show (ie sketch icon in design tree highlight blue)
Unfortunately, turning off sketches in the 'show hide items' menu affects flat pattern bend lines on drawings, so must be left on. We use sketches for etchings and scribe marks as well, so they must be shown. Additionally there are bugs in the software (specifically in relation to configurations) where sketches show themselves. For example, I just added a flatten feature, a sketch to load the flat overalls into the DT, and a fold feature. After these operations, sketches are automagically showing. This is a consistent, easily reproducible bug. These bugs have been present for at least 10 years. What needs to happen is to give us control of the show/hide state within a config table. Turning off 'Link display states to configurations' seems to be the easiest way, but it is completely unintuitive (not to mention all the baggage associated with carrying all those display states). The whole SW display state design is a huge failure in my opinion. Very few people use them because learning them is completely unintuitive. This is a prime example.
OK, maybe someone mentioned this already, but make sure that "Link display states to configurations" is Unchecked.
Then in the box at the bottom of your configuration manager area, delete all display states except one.
Hide that sketch.
Now that you only have one display state, it is hidden in all configurations.
Or alternatively, you could activate each display state and hide it in each one.
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