I am trying to make detail drawings and reference back to assy drawing to help the partsmakers understand the assy. Is there an easy way to do this? Thanks
Our Drawings have 2 lines for the title, the first name is the Assembly that this drawing is a component of, and the second line is the name for the part. In the drawing of the actual Assembly, the second line is General Assembly.
I thought maybe I can create a new drawing document of the assy, inserting a BOM, then insert a new sheet containing a Part detail and simply insert a balloon refering to the assy BOM. Is this possible? Thanks
OK, if I understand you correctly, you have an assembly on sheet #1 with a BOM. You want to put a part detail on sheet #2 with a balloon that identifies that part back to the BOM of the assembly on sheet #1.
Here is how you can do it:
Method #1:
Make a configuration of your assembly that HIDES all components but the one you want to show on sheet 2. Use that configuration of the assembly when inserting a view on your sheet #2.
Method #2:
Inserert a view of your assembly on sheet #2. Then, in the drawing, hide all the other parts you don't want to see on sheet #2.
If your item bubbles are driven by the BOM, you will have to make the item bubble balloon text "Custom" instead of "Item Number".
I've done it the way Arlin has and it works fine. I have also hidden the components within the drawing view, but this can eventually made your drawing file large, especially if you have multiple sheets pulling out details.
I favor adding my 2nd sheet, inserting the actual part, and detail it just as I would if it were a detail machine drawing. I change my item bubble to a color that stands out (like red if all your bubbles and notes are black). Also set my BOM properties to reserve row numbers for missing components, so when the BOM updates, I don't have to change my item bubble number. But the red color is a good indicator to verify it. This works great for weldments, since we have a job shop do all this for us.
Hope this gives you the option you were looking for. Good luck!
I have made a several weldment drawings that are similar to what (I think) you are describing. These are basically nothing more than an assembly drawing with all of the parts documented on the following sheets. I do use a special BOM for these drawings and I am careful about the part number and description. What I want is to have all of the 1x1 - 2x2 – 3x3 - etc parts listed as 1 item each. Other parts like weld-nuts or studs are also listed on the BOM.
There is nothing that says every view in a drawing has to refer to the same model. My first few sheets normally refer to the weldment assembly, but the detail views directly access the part file where they are defined.
The problem I have is that I have about 10 sub ass'ys cosisting of about 110 parts. My files would be huge. I guess having a link to the part name that cooresponds to the BOM might work to keep track of the parts. Then the only problem is if I have two or more parts on one drawing, I'll have to do some manual typing.
Thanks
No – With that many parts you would not want to do it that way.
Have you tried doing this with Custom Properties? If all your looking for is a way for your part drawing to reference the assembly where it is used, then this shouldn’t be all that difficult. What you would need to do is add a Custom Property to each part in the Assembly and give it the Assemblies Part Number. You could then add a text link to the CP in your drawings Template file. The text might say something like “Used On: 12321-101”
To add the CP in the part files, write a simple macro and attach it to a macro toolbar, then in the assembly open each part – and click the button. You can have the macro save the file and close it so all you’ll need to do is a single click. If you need help with this I will modify one of mine for you. You would need to edit this file to change the assembly number before processing another assembly.
With a little more work, you could also make the macro recursive so that it operates from the assembly level, opening each part file and adding the CP. There are 2 problems with this. The first is that you would have no control over which files the CP was added to – every file would get the CP. The second has to do with a part that is used in multiple assemblies. You would have to decide how to handle this. The macro would either – 1- ignore the CP and do nothing 2- replace the CP 3- append the new assembly to the CP. While the last option sounds like the answer – if the macro was ran twice in the same assembly every one of your files would end up with multiple entries like: “Used On: 12321-101; 12321-101”
