New BOM for multiple drawing views

[pdybeck]

I have a assembly drawing with the new BOM. One view is of an exploded config of the assembly model, and another view is of a section cut of the same assembly model. I inserted the BOM based off the exploded view, but can't seem to get the balloons on the section view to match the items in the BOM. If I go to properties on the section view there is an option to link to the BOM in the sheet. I check that option, but as soon as I insert a balloon on that section view, that option is automatically turned off and the balloon does not match the BOM. It seems as if this function is broken. Can anyone confirm this? Is this a bug? I am working with my VAR on this, but would appreciate extra info. I do not want to go back to using the Excel based BOM.

Pete Yodis
Harold Beck and Sons

 

[SBaugh]

I tested just this using SP2.1 and it works fine here.

I have an exploded ISO view, a front view and a section view (taken off from the front view). I add the BOM using the Exploded ISO view. I used Auto insert of Balloons for the ISO view. That worked fine, but some of the model items were still hidden and didn't show up in the exploded state. So I added balloons to the Section view using the same function (Auto Balloon). It showed the parts that were hidden with a balloon. I then started adding Balloons manually to make sure they corresponded to the BOM. Which they did without a problem. The option in the Section view "Linked to BOM" was checked by default.

So I don't see this as a problem. Make sure that link is checked and try removing your BOM and re-adding it and see if that makes a difference.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[pdybeck]

Scott,

My Section view was created on the model as an assembly cut and stored as a different config. I wanted to show an isometric section view. The exploded view is a different config than the section cut. A little bit different than creating a section view on the drawing, but I needed to show it in isometric view.

 

[SBaugh]

That's is needed information to do a proper test. I'll try it again and see what I get.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[pdybeck]

In the meantime I am creating a section view using the new section tool on the assmebly model. I will save that view of the model. Then on my drawing I will change the config being used on the original section view to the same config that was made for the exploded view and pick the section view I saved in the model. Hopefully you follow what I am saying. I'll get back to you.

 

[SBaugh]

Ok I made a Configuration that has an assembly cut, and it cuts every part in the assembly. I placed that configuration into a view onto the drawing. I added manual Balloons to the view and it corresponded to the BOM like I would expect it too.

Have your tried checking that option and then removed your BOM and re-added it?

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[pdybeck]

My other idea doesn't work. The section isn't saved when you try to view it in the drawing.

 

[pdybeck]

Scott,

I tried your suggestion. No luck. If I go to the BOm and Add the section view as another config, then the item numbers change to match in both views. This happens in real time. I can check and uncheck the section config in the BOM properties and I can see the balloons changing back and forth from matched to unmatched. This happens with more than one drawing of ours and I think I have found a bug. I don't want to have to add the section config to the BOM under its properties because then I will have two quantity columns, one for the exploded config and one for the drafting config. Definitely seems like something is wrong, because I can repeat this on many drawings. Also, not all items are unmatched, just a few. You might want to try this test with a larger assembly that has more components.

 

[SBaugh]

FYI to all here if you curious about this post - I talked to pdybeck offline on this subject. I found that he was making the section view as Derived configuration. For some reason when it is a derived config it does fail like Peter pointed out.

The workaround however is to make a configuration. Not a derived one, but an actual configuration. Once you do that update the drawing view in question the BOM balloons update accordingly.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[captaincaveman747]

hello out there I am having the same problem as pdybeck but I have a slightly different variation. I have a left and right hand assembly of a door frame w/ metal skin. The RH config has a derived config for the drawing file (ballooning). In the assembly there are 3 configs of 1*2 tube (different lengths). They show up fine in the BOM=separate numbers but the balloons show up with the same number.
Your suggestion of creating a new config and not a derived config will not work for an exploded view. Any help would be appreciated.

 

[SWCADMAN]

Hello,

I'm having the same problem...I have an assy with 2 cfg's. The drawing is 2 sheets. The BOM table is on sheet 1 with one of the cfg's. Sheet two has the other cfg. What I want is to have 1 BOM for both cfg's with only one QTY column.
Thanks in advance for any help.

SWCADMAN

 

[pdybeck]

Good luck. The new BOM is still buggy for things like that IMO. I haven't found a sound method to make sure that both configs use the same BOM and that there aren't issues with the item numbers. Also, I have problems with the order jumping around alot when we edit the BOM. When you have a 50 item BOM, this gets to be a real pain real quick, especially when you have more than one drawing to do. A simple addition to a BOM can end up taking way too long. I have noticed that when you group items together, lock the BOM from changing item numbers, and then you go back and unlock the BOM - all the grouping is destroyed. Real pain in my A**. I am acutally checking out 2005 Beta for things like this that end up eating up time in my company. A complete loss of ROI (to use SolidWorks marketing language) when considering upgrades. If things like this that cost users so much time (money) aren't fixed, then whats the use of paying subscription? What is the money really doing for us?

Pete Yodis

 

[shenzy]

service pack sp4.0 fixes this thank god.
You still have to go into the views properties on the
drawing and check off the link BOM button and point to the current BOM name. Much nicer

 

[pdybeck]

Yeah! I heard this the other week and its about time. Seems like the functionality was thought out, just never completed. There are still other improvements that need to be made - things like the order of the BOM shifting around dramatically when it is unlocked and when grouping and un-grouping items. All in all this is a step in the right direction.

Pete

 

[ryanmech]

Is it possible to have several views of several different parts/assemblies listed in the same BOM.

Previously we have just had one assembly per sheet, and its particular parts detailed in the same sheet with the BOM derived from the single assembly. What about if we have random parts/assemblies on one sheet, can they be all on the one BOM

Thanks
Ryan

 

[SBaugh]

You can have multiple assemblies on one sheet, but each assembly will have to have it's own BOM. They all cannot read into the same BOM.

FYI - This should be posted as a new question post, instead of being asked here. You can always copy this thread559-89101 into a message.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users