Balloon trouble

[gareth01422]

Hi all

I am seeking some help with an assembly I am trying to detail up at work.

The assembly is 4 pipes (flanged at each end) and 5 layers of lead rolled around the pipes. All the pipes are different lengths, so to create the lead shielding I created 4 parts with configurations for the different lengths. This is also table driver. In the assembly when i take a section view and try ballooning the view up, it keeps putting in silly numbers like 134, 112, 126. when there is only about 60 part on the BOM. I am also using 2010 version if anyone needs to know.

any advice welcome.

Gareth

 

[Nella95]

Have you tried a 'hard update?' (ctrl-Q) - both on the drawing and on the solid model - also with each configuration active. (This might help - more a 'shot in the dark' than anything.)

 

[CorBlimeyLimey]

Was the section made in the assy model or the drawing?

Can you post a screenshot showing the balloons, the BOM and the BOM Property Manager?

 

[NL8]

If there are multiple views from different configurations that you want to reference the same BOM you need to link them to that BOM. RMB on the view with the messed up balloons, choose properties, then look in the bottom left hand corner. There is a check box that should say Link to BOM and a drop down that will let you pick the BOM to link to. Make sure the box is checked and is pointing to the BOM that has the numbers you want. All should be fixed then.

Joe Hasik,
CSWP/SMTL/MTLS
SW 10 x64, SP 3.0
Dell T3400
Intel Core2 Quad
Q6700 2.66 GHz
3.93 GB RAM
NVIDIA Quadro FX 4600

 

[gareth01422]

Brilliant DekkerDesign

It worked great, There were 3 BOM lists in the drop down menu so only took a few minutes to sort out.

Thanks again guys for all the help.

Gareth

 

[moyesboy]

This one is annoying, I spent a long time on the help line to arrive at the solution posted here.
Any new view should be linked to the BOM if there is only one bom, by default. Who would want it not to be?!

 

[NL8]

Typically if there is only one BOM in the entire drawing file there isn't an issue. I've only seen this problem when the software needed a repair or when there are multiples BOM's in one file. Mind you, I say in one file, not on one sheet. I've noticed similar behavior with putting multiple copies of cut lists for weldments in one drawing file, but there's no way to correct it.

Joe Hasik,
CSWP/SMTL/MTLS
SW 10 x64, SP 3.0
Dell T3400
Intel Core2 Quad
Q6700 2.66 GHz
3.93 GB RAM
NVIDIA Quadro FX 4600