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Hawk Ridge Systems is a global provider of engineering design solutions that radically improve the way our customers design, develop and manage their product life cycle.

Make a Universal Weldment BOM Template Using Nested IF Statements

 
May 23rd, 2014 by Hawk Ridge Systems

Universal Weldment BOM Template

Suppose you want to make a SOLIDWORKS Universal BOM Template for mixed weldments which incorporates weldment structural members but also sheet or plate and even purchased parts. Suppose you also want to automate the BOM as much as possible to avoid manually inputting data and have it update parametrically with changes in your design… How do you accommodate the three different types of components so that manufacturing knows which materials to use, and accounting can quickly add up the material costs?

Universal Weldment BOM Template

Using nested IF statements in your BOM columns, you can do just that. For the BOM above, the only values which require manual input into the parts are Part Number and Description. Description should already be defined at the profile level for all of your structural members anyway. None of the cells are being managed manually at the drawing level, which is as it should be for a parametric CAD tool.

To do this, just create a weldment using structural members as you would normally, but make sure that you are creating any sheet metal or plate parts using the Base Flange/Tab in the Sheet Metal tool instead of a regular Boss/Base Extrude. We also recommend that if you commonly use flat bar in your designs that you create custom Weldment Profiles and create those parts as structural members. Update your cutlist, and give each cutlist body folder a custom property called PART NUMBER. Description will automatically be filled out for structural members, and for the plate components; we recommend copying and pasting the Value/Text Expression from the Sheet Metal Thickness property followed by your unit of measure and “PLATE”, so that the thickness updates parametrically with design changes (see below).

Universal Weldment BOM Template

Now, put your model into a drawing and add a Bill of Materials using the BOM-standard template that comes with SOLIDWORKS.  For BOM Type, select Indented with Flat Numbering and check the Detailed Cut List checkbox. Right click the column header for QTY, and insert a column to the right. Select “LENGTH” from the custom properties drop-down that appears. Repeat this process to create columns for BOUNDING BOX LENGTH and BOUNDING BOX WIDTH.  Also create two more columns without selecting a custom property (just click in the paper space when the dialog pops up) and title these USAGE and UM.

At this point, since we created an indented BOM instead of a weldment cutlist, there will be a top-level row for your weldment file and any other top-level components (if you are working with an assembly instead of a single part). The assembly used in this example consists of the main weldment, threaded base plates and the leveling legs. If you want to keep the top-level rows in your BOM and give them custom properties, remember that these are coming from the file->custom properties menu, not the cutlist since these are top-level components. Also, you can change the “flat numbering” style we specified earlier to “detailed numbering”.  This will change the numbering scheme to 1, 1.1, 1.2, etc. for the top-level components and all subcomponents.

If you don’t want these rows in your BOM, you can simply right click on the row and hide it. Alternatively, you can expand the BOM with a left click on the three arrowheads on the left and use the minus sign or dissolve command to properly condense them.

Universal Weldment BOM Template

If you have filled out all of the DESCRIPTION and PART NUMBER fields at the model level, they should be correctly displayed on the BOM. QTY is also calculated automatically. All of your structural members should have a LENGTH, and all of your sheet/plate components should have a BOUNDING BOX LENGTH and BOUNDING BOX WIDTH. (Note that you can use Bounding Box Area, too, but we prefer length and width because this tells the fabricators the dimensions for each piece.)

The last two columns are the real secret to the universal weldment BOM template. Here we will be using a nested IF statement to differentiate between the three component types. Left click on the column header above USAGE and click on the summation sign (Σ).  This will open the equation editor and we will be applying the equation to the entire column.

Universal Weldment BOM Template

Enter into the equation editor:

IF(‘LENGTH’>0;’LENGTH’*’QTY.’;IF(‘BOUNDING BOX WIDTH’>0;’BOUNDING BOX LENGTH’*’BOUNDING BOX WIDTH’*’QTY.’;’QTY.’))

This is telling SOLIDWORKS that if the component has a length, it is a structural member and should calculate total usage based on the length times the quantity. If it doesn’t, it is either a plate/sheet component, or a purchase part. If it has a bounding box width, it is a sheet/plate component and total usage is the length times the width times the quantity. If it’s neither, it must be a purchased part, and we just report the quantity. We do something similar for the Unit of Measure (UM) field. The equation for the Unit of Measure is:

IF(‘LENGTH’>0;”IN”;IF(‘BOUNDING BOX WIDTH’>0;”SQ IN”;”EA”))

Here we are just outputting text values using the same test criteria. When creating equations in SOLIDWORKS BOMS, it is easiest to use the drop-downs in the equation editor, but if you want to create them on your own, notice that Custom Properties are bracketed in forward apostrophes (`Custom Property`), a Column is bracketed in regular apostrophes (‘Column Name’), and Text is bracketed in quotations (“Text”).

The last step of course is to save your BOM as a template. Left click anywhere on your BOM, right click on the black arrows in the top left of your BOM, and select “Save as”.  Save it as a SOLIDWORKS BOM Template (.sldbomtbt) somewhere other than your install directory (so it doesn’t get written over with the install of next year’s version of SOLIDWORKS), and it’s ready to use for all your upcoming weldments.


Hawk Ridge Systems Engineering Team

Hawk Ridge Systems Engineering Team

It often takes a team to solve a problem – and sometimes it takes a team to write about it.
The Hawk Ridge Systems Engineering Team is comprised of our Product Managers, Applications Engineers, and Support Engineers. They’ve collaborated on this blog entry to bring you the most accurate information about the solutions you use for design and manufacturing.

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Category: SOLIDWORKS 3D CAD

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