Working our Alignex support hotline, I have received these SolidWorks questions on multiple occasions:
"I have some components that I want to show on my assembly drawing as hidden or reference. Additionally, I do NOT want them to show up in my Bill of Material. How do I do this?"
In an effort to provide the answer to a wider audience, I'm posting it here on our blog.
1. If you don't want Components to appear in your Bill of Material, select the component's properties in the assembly tree. You will find a checkbox in the lower right corner of the window that will allow you to "Exclude from bill of materials".
2. To show the component in a drawing view using a different font, Right click on the component in the drawing view of the drawing tree. Select component line font and uncheck the box to "Use Document Defaults". Choose Phantom (or other font) for ‘visible edges'.
3. To hide the component in your other drawing views, add the component to the list on the hide/show components tab of the drawing view properties by selecting them in the graphics window when this dialog box is displayed.
Tim Mika
SolidWorks and SolidCAM Application Engineer
Alignex, Inc.
tmik@alignex.com
Here is a neat way to control the QUANTITY of your weldment members in a top level ASSEMBLY Bill of Materials:
First begin by using the new ‘dissolve weldment' command on your assembly drawing BOM:
This may put in the actual weldment members LENGTH in the QTY column and cause you to stare in disbelief at the values for QUANTITY!
Simply open the WELDMENT PART in its own window, expand the cut list in your feature tree, right click on each of the yellow folders and pick ‘properties':
Here you can set the BOM Quantity to -none- for each item....Your BOM will now look like this:
Another great reason to use the weldment tools in SolidWorks!