As the title says, when I insert a BOM in a drawing from a assembly the lenght column is empty.
What can I do?
Are you talking about a cut list from a weldment or BOM from an assembly?
In a cut list, the length has to be defined in the properties for each cut list item and the column in the cut list must be linked properly.
Yes, I'm talking about cut list. My tree is like this:
I started a drawing from the assembly. I defined lenght at properties in the part, and the column is linked properly.The value doesn't appear.
So you are adding a BOM to a drawing based on an assembly that contains weldments? If so, then you need to have the BOM type set to Indented with the Detailed cut list check box checked. See my attached picture.
Ryan, I don't want to show the item numbers like detailed cutlist, I need sequencial numbers.
I saved the template and when I insert the table in the part, the value is there. It should work in assembly...
Because is illogical insert a table for each view of the same part... If it's like this, it's better to write the value manually...
2. Suppose that you have a rectangle and make a structural member using the same type. In BOM, I have the verticals and the horizontals separated, but I need them together, with the lenght an weight added, and using the same item number. Should I do this manually in the table? Any other suggestions?
I'm having a LOT of difficulties to make the drawing of weldments in SolidWorks, specially the BOM. I already lost all the time I had for finishing the project with this kind of stuff. I'm considering to return to AutoCAD to do the next project, and in this one make the table totally manual in SW.... This is really sad
Are you creating the drawing for a weldment using an assembly? I am sorry but I am just not sure why you are using an assembly to try and detail the items in your cut list. This is much easier done just using a drawing and cut list based on the weldment. What is your reason for not doing it this way? Maybe I can help you there.
You can change the BOM I showed above from Detailed numbering to Flat numbering.
A section view can be linked to a BOM if the balloons are not appearing correctly.
In a cut list the items will appear as the same cut list item if they are identical. If they are not showing up the same than something in the modelling is keeping them from being the same. In your case, in a rectangle you must make sure you are trimming them so that all the lengths of the pieces are the same length otherwise the horizontal pieces will be different from the vertical ones.
1. I'm using an assembly to create the drawing of a weldment because I need to show the other parts in grey. And for this, I'm using layers in the views.
2. How to link a section view to a BOM?
3. And for the other problem, verticals and horizontals are always different, but in BOM I need to have only one number item for each "type". For exemple, if I have 2 thousand of C channel 3x5, I don't want 2 thousand itens in my BOM, but just one, no matter if the lenghts are different.
1. What other parts? Maybe a screen shot of what your drawing looks like will help me understand.
2. See attached picture.
3. SW is a parametric program so what you are trying to do is kind of flying in the face of what the program is meant to do. It is designed to recognize parts that are the same and report them as such whether this is in an assembly or a weldment. Manually manipulating things is an option.
1. Take a look at the picture.
(What is black is what I need to detail and show in the BOM, and what is grey is a kind of reference)
3. Talking about drawing and manufacturing, It's weird to have a same kind of shape, with the same material, separated only because they have different lenghts, and with different numbers in the balloons. It' would be nice if I could choose If I want all the same shapes added or not. I have a weldment here that has 8 bodies of the same 1-1/2" pipe that are separated in the list, and to show the total lenght of them and to show balloons with only one number for these bodies, I need manual work. And the worst is that the table doesn't work as an excel one. There are things that are easy to do, but others are complicated or impossible, or have bugs. SolidWorks' tables are too precarious.
I see what you are doing. I will be honest and say that how you attempting to do this is not how weldments in SW are really meant to work. That doesn't mean you can't do it this way but you are definitely going to be restricted in how you do it.
You have 8 separate bodies because they are 8 unique pieces. That is the whole point of a weldment. To either combine or separate pieces based on their geometry. The way a weldment is meant to work is to detail each of those eight pieces in the same drawing as you show how to assemble them. Technically a worker can then gather his material, look at his drawing and cut each to length and prepare them as necessary to weld together.
Yeah, maybe you're right.
I'm gonna change the way to present the project. It's easier for me, and more detailed for the man who will manufacture the piece. I'll have a bigger table, and probably I'll have to use one more drawing because of this but c'est la vie...
Guess I'll take off this grey reference and work with the part. And then I can make an exploded view to show the positions of the parts.
Thank you for the support Ryan!
I couldn't agree more. You may need to create an extra assembly drawing to show how it all comes together but I can pretty much guarantee that it will be much easier for you this way and as you said it will give the people putting it all together better details and instructions.
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