Part configurations in Balloons/BOM 2

[mkmech]

I have an assembly in which there are several instances of a given part. Each instance is a different configuration of that part. I have created several configuration-specific properties for that part. Now when I make a drawing of that assembly, I want to show each instance (configuration) by a separate balloon and consequently, this should appear in the BOM accordingly. However, when I put a balloon on these instances, they all get numbered the same, which means there is only one entry in BOM for that item number. What I want is each instance (Config) appear as separate entry in the BOM with their corresponding config-specific value.

How can I fix this problem? I tried searching through the forum for this and did find a few related posts but none of them addressed this specific problem. Also, it would be great if I don't have to create any Excel macro as I don't know how to do that.

Thanks to all the readers

 

[CADGemini]

You need to go to each configuration of that part and right click on it. Go to properties of that configuration and tell it to use configuration name. Or you can tell it to use user specified name.

Now solidworks will recognize each part as a aseperate line item in the BOM.

Best Regards,
Jon

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

 

[mkmech]

Thanks jksolid. It worked.

A few more questions:

1. I want to have 2 BOMs in the same drawing. The reason is that I want to lump parts into 2 "groups" and have a separate BOM for each group. The item numbering in 2 BOMs will be different and so will the columns. For example:

BOM1:
Item numbering is like 1,2,3,4,5...
Columns are: Item No, Part No, Part Description, etc.

BOM2:
Item Numbering is 101,102,103,104,...
Columns are: Item No, Description, Cut size

I will be making balloons that reflect this 2 different numberings.

I have already created 2 cutom BOM templates that have the respective columns. I did manage to insert 2 BOMs but they don't look right. For example, the balloons corresponding to 2nd BOM don't have numbers like 101, 102,.. even if I double click the balloon and change the number to 101 or 102, it goes back to 7,8,9,... I already cleared the "Row numbers follow assembly ordering" check box on the Control tab of the Bill of Materials Properties dialog box.

Any suggestions?

Thanks to all

 

[CADGemini]

As far as I know I don't think you can have two BOM's driving the same drawing. However you can insert the two BOM's like you have done already and when it comes to numbering the 101,102,103, etc. numbers all you have to do is right-click on the balloon to get the balloon settings. Change the size to 3 characters. And balloon text should be set to custom and in the value box type in 101, 102 etc.

Doing this method will not automatically update the custom balloons.



Best Regards,
Jon

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

 

[mkmech]

Thanks jksolid. I am now able to custom number the balloons.

But I still have one problem left - as I mentioned in an earlier post, my intention was to have 2 different BOMs in the same drawing so that I can have different columns for different parts. That is, in BOM1 (Item No, Part No, Part Description, Qty) and in BOM2 (Item No, Cut Size, Qty). Then I would like to have the parts that have the corresponding properties go into the corresponding BOM. Is this possible in any way?

Thanks to all.

 

[CADGemini]

Sure it is possible. You will have to create a custom BOM with custom properties that match the properties in your parts. It would take awhile to discuss each step in doing this.

You could for instance have a solidworks generated bom for the BOM1 and delete columns you don't need.

For BOM2 it looks like you will need to have a custom made BOM made in excel. You then can insert- object-from file and browse to the excel BOM you made. Look in SW help under Creating Excel based BOM's

I hope this helps!


Best Regards,
Jon

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

 

[cninneman]

I have a question on the first topic. I want just the opposite of what was asked. I have 2 configurations of a part, a right and a left, I want them to show up as one line item in the BOM with a qty. of 2. Each configuration is set to use the "Document Name" and by default I got two lines, qty. 1 each.

What have I done wrong?
Chris

 

[TheTick]

What disturbs me about this is that this is not how the BOM is supposed to work. If any config-specific properties used in the BOM are different, they components should be treated like separate parts (this is documented in the help file).

Of course, that begs this question:
Even though you have assigned configuration-specific properties, are those property entries actually different from one another?

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[engAlright]

Cninneman-

As I understand it, to fix this you have to set each configuration of the part to use "user-specified name" in a BOM. Probably easiest to do this with a design table that includes the $partnumber header, then the value for each configuration would be the partname you want to appear in the BOM.

The second part of the fix is on the Bom Properties, under part configuration grouping, to select "Display all configurations of the part as one item".

This seems like a roundabout fix to me, but apparently Solidworks says this works as it is designed, which I don't fully understand as I can't think of an instance where you would want an item listed twice in the same BOM with different item numbers. I would always assume that any documents with the same name will appear as a single item in the BOM.

If anyone has a better fix, I would love to hear it.

 

[cninneman]

The deal is this, normally I would do what you suggest. But, this is a case where it's a simple routed cable (swept feature), one routed left, one routed right. They are, for all purposes, the same part, just routed differently. I didn't want to make two seperate parts, because it would definately be seen as two line items, so I thought configurations was the way to go. Untill I saw how it appeard in the BOM anyway. The part does not have config. specific properties, just one set of custom props.

Am I doing something wrong? Is there a better/smarter way to do this?

Thanks
Chris

 

[cninneman]

engAlright,

Thank You!! That's what I was missing. I just needed to click the button for "Display all configurations of the part as one item".

I agree, it seems odd that it would require this, but as long as it makes my bill work, I'm ok with it.

Thanks again
Chris