Ballooning issue with revolve...

[mx2street]

I'm trying to balloon an exploded view and everything else will accept an item numbered balloon except this little o-ring which is just a sketched circle revolved. Any ideas?

 

[SBaugh]

Is it a true part then? or just a sketch? - It's just a sketch then you should probably make it into a solid.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[mx2street]

Yes, it's a true part, solid body and all. I even tried putting a little square (.05 x .05) in the middle so it would maybe have a flat face to attach to.

 

[CADGemini]

What version and SP are you running? Try upgrading to the latest SP. There were some fixes with the balloon feature.

Another thing to try is to open the assembly in the exploded state and also open the O-ring. Do a Ctrl+Q on both items and save them. then open the drawing to see if you can now balloon the O-ring.

Sometimes with exploded views the part becomes invisible on the drawing because you either modified the exploded view for that item or you replaced that item with a different one. Using the Ctrl+Q method has worked for me.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

Solidworks 2005 SP3.1

 

[ctopher]

You need to open the oring part and add a "split-line" so you can dimension it and/or add annotations.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site

FAQ559-1100
FAQ559-716

 

[mx2street]

Chris, that worked pefect! Thanks everyone for the help, new shortcuts are always good too.

 

[CorBlimeyLimey]

In SW04 you could place a balloon or annotation on the surface of an o-ring (or non-planar face) without need of a split line, etc. Has this changed in 05 & 06?

I suspect that by adding the split line into the o-ring, you effectively did a rebuild (per jksolid) which updated the exploded assy.


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[ctopher]

In 05, if there is cylindrical part, it sometimes creates a silhouette. Create a split line on the cylindrical part to solve some drawing issues.
I do not recall having this problem in 04.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site

FAQ559-1100
FAQ559-716

 

[Regg]

The problem mx2street describes was in SW2004 too. Have not used SW2006 enough to know if it is there. I was able to solve the problem by using a method similar to jksolid. First open the assembly and make the configuration being ballooned active. If that did not work, set the configuration to the exploded state. Still did not work, then open the part. If the part would still not balloon, then I would use autoballoon. At least one of these always seemed to work.

Regards,

Regg