drawing gremlin

[Istre]

Ok, lets see some of those big brains on this. Here's my problem, I have an assembly and I'm drawing up the prints for it. In one particular isometric view, there is a part that is clearly visible in the print, yet when I go to add a note or a callout with a leader to that part, SW refuses to acknowledge the part is there and attach the leader to it. I can hide or unhide it, suppress and resolve it, but in the drawing window proper, SW just refuses to believe it's there.

I've had this problem before, and I hope some of you have as well and can tell me what's causing it, because it's driving me nuts.

Thanks a lot, folks!

 

[ShaggyPE]

I have experienced this as well. The last time I remember it happening was when I was dealing with an exploded view. I could never get it to attach correctly. I just settled for a brown balloon and a custom number.

 

[ctopher]

I think we all experience this. Some tricks that sometimes work is ... zoom in/out and try attaching the notes, change scale of view then try, or save and close SW then reopen and try.

 

[SBaugh]

Have you tried highlighting the view and doing an Insert Model Items on it. Insert all dims, to see if SW recognizes it at all?

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[Istre]

Hmm, that's a good idea, SBaugh, but I'm trying to insert new notes with leaders to the part in an assembly. There's not a lot on the assembly itself to insert with Model Items, and nothing on the part in question.

 

[SBaugh]

I'm just testing the waters to see if SW Recognizes the view at all. I understand your trying to add a note. So try adding something other then a note, like a Weld symbol, surface finish symbol, balloon, etc...

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[Istre]

Basically, it's as if the part doesn't exist. Anything in front of the part is selected, as usual, when pointed to, but anything behind the part is selected as well. Turning off surrounding members or supressing them doesn't help. Then it just doesn't select anything.

 

[Istre]

Ahh, I didn't say that at the beginning. Yes, I am trying to add a note, but nothing else works either. I can't select the part just by clicking on it with no function selected. Balloons won't attach to it, I can't put a weld on it because I can't select it. I can't dimension it because it won't select any part of it. It's as if it's a ghost in the drawing window, but present in the feature manager

 

[Istre]

I just noticed something else. I have two parts that are behaving like this, and both of them have multiple solid bodies.

 

[CorBlimeyLimey]

Can the bodies be merged?

 

[SBaugh]

Try deleting the view and readding it. It's not a custom or named view by chance is it?

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[Istre]

Actually, it is a custom view created through a macro. I modified the 8-iso macro to also produce 8 dimetric and 8 trimetric views. However, this problem has occured before I began using this macro.

 

[Istre]

Ok, I found out a way around it, so someone might be able to come up with the reason why this is happening. Basically, if I make the view unexploded, I can select and point to the part. If I were to make the view exploded, the leader stays stuck to the part, but I can add no new leaders, and I can't select the part anymore until I revert back to the unexploded state.

Thanks to everyone for their input and help.

 

[ctopher]

You didn't say initially it was en exploded view. It acts the same as a broken view, it needs to be unbroken to add some dimensions. So, unexplode to add notes/dims.

 

[Istre]

Yeah, I forgot that tidbit of info. What throws me for a loop, though, is that some parts will allow themselves to be annotated on and selected in the exploded view, but others won't, and I can't figure out how they decide which is which.

 

[CorBlimeyLimey]

Could it be the parts which haven't moved can be annotated?
Or perhaps those moved in a certain direction which can't?

 

[Istre]

Ok, last update to this thread, I promise. I think I've figured out what's going on here in case anyone cares. When you have a drawing view in a drawing document that is shown in the exploded state, it appears that any part that has sketch references to another part reverts to a state in which it cannot be selected. Once the assembly is collapsed, it is once again in context with its references and can be selected.

Hope this helps someone.