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Dialing it in - Using TolAnalyst on Your Assemblies, Part 1

Vince Farrell

This article is the first part of a series about how TolAnalyst (available in SOLIDWORKS Professional and Premium) can help you in your assembly and part design. In this first article, I’m going to go over DimXpert and how it works with TolAnalyst, but before I get started, I want to share an anecdote from my days as a designer. As embarrassing as it is, in my time in the industry, I know I’ve been called into my bosses’ office where we’re standing over the actual prototype of the machine I’ve been working on for the past weeks inside SOLIDWORKS. My heart was beating with excitement as I’m looking at this masterpiece which, up until then, I’d only seen on my computer screen. However, my heart descends down into my stomach as I look at my bosses’ face and he tells me, “It doesn’t fit together.” My first thought is, whoever made this messed it up! Upon further inspection, unfortunately, it’s my fault because everything was made per print and my tolerance stack up was off. Enough airing of my dirty laundry, let’s go into how to avoid this situation.

Picture

To start with, here’s a summary of what TolAnalyst does. This is an add-in that will take into account all of the tolerances in your assembly and create a tolerance stack up. Once you have your analysis results, you can modify the individual dimension tolerances so that the parts always fit together. Pretty useful, right? To start TolAnalyst, eitherClick the arrow to the right of the System Options, select Add-Ins and Select TolAnalyst or use the SOLIDWORKS Add-Ins Command Manager to turn it on.

SOLIDWORKS

The reason that I want to go over DimXpert in this series is because TolAnalyst uses the data from DimXpert to complete its tolerance analysis. You can use DimXpert to either add dimensions manually or automatically based on the type of part. I’m going to use DimXpert and TolAnalyst on this sheeter assembly.

SOLIDWORKS

This sheeter has two knives that move up and down, cutting the sheet. As a designer, I don’t want the blades to be too close together because they’ll crash, and I don’t want them to be too far apart because they won’t cut the sheet. Therefore, I’m going to use TolAnalyst to make sure that I don’t get either of these situations.

The first thing I need to do is to make sure DimXpert has been applied to all of my parts. I’m going to use that on the upper knife block, but to start with, I want to show you a simple part just so you can get a feel on how DimXpert works. Here is a simple block with two of the same size holes.

Block

I’m going to go to the DimXpert Manager tab on the Feature Manager and start with an Auto Dimension Scheme.

SOLIDWORKS

In the property manager, I’m going to pick the following options: the part is Prismatic, not turned, and I want to use GD&T to dimension it. I just need to pick some datums, tell SOLIDWORKS the features scope and hit the green check. You can see the colors of the faces that I’ve chosen match the Primary, Secondary and Tertiary datums.

SOLIDWORKS

SOLIDWORKS adds all of the dimensions based on my datum selections.

SOLIDWORKS

If I’m not happy with the tolerances that were automatically applied, I can always go up to the Document Properties and change tolerance amounts on different dimensions. In this case, everything looks pretty good and DimXpert even picked up that the 2 holes are identical and added a 2X to that dimension. If it didn’t, I can fix that by CTRL selecting both dimensions, right clicking and hitting Combine Dimensions.

I can also import all of these dimensions to a drawing so I don’t have to do double work. After creating a drawing from the part, in my View Pallette, I can click on Import Annotations and DimXpert Annotations.

SOLIDWORKS

Drag and drop one of the views with an “(A)” next to it. Just like that, the DimXpert annotations are included on the drawing view.

SOLIDWORKS

If you have those options off, you can still bring in these dimensions. Just click on the view and turn on those annotations in the Property Manager. Note, if there isn’t an “(A)” next to the view in the View Pallet, there aren’t annotations to bring in so nothing will happen if you turn that on.

SOLIDWORKS

Back to the sheeter, I happen to know that DimXpert hasn’t been applied to the upper knife block, so let’s do that using the same steps that I used on the simple part above.

SOLIDWORKS

There is one change that I need to do. The holes are supposed to be press fit for a bushing, so I’m going to change the tolerance to a tolerance with fit and make them a P7 press fit. I do this by clicking on the dimension and changing the Tolerance/Precision.

SOLIDWORKS

With my DimXpert dimensions applied, I’m ready to start TolAnalyst. However, that will be continued in the second part. If you prefer, you can see my YouTube video here. Thanks for reading!  

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