Welcome to my second article in this series on using TolAnalyst for assemblies. In this second article, I’m going to set up a tolerance analysis so that you can see what’s involved. Before going any further, if you haven’t done so already, please read Part 1 of this series. Go ahead, I’ll wait… Okay, now that’s out of the way, let’s go back into this “sheeter” assembly. All of my parts have DimXpert dimensions and tolerances, so I can start my TolAnalyst study to make sure the knives don’t bind together and aren’t too far apart. In this case, over ¼” apart would be too far because the assembly won’t cut a sheet at that point. There is a 4 part process to our study:
- Define the measurement you want to control.
- Define the assembly sequence.
- Define the assembly constraints.
- Run the analysis and adjust the tolerances as necessary.
This article will cover Steps 1 through 3, and the last article in the series will cover running the analysis and refining the results. To start the study, click on the DimXpert Manager tab and click the TolAnalyst icon. (Remember, if this isn’t available, make sure that TolAnalyst is turned on as an Add-in.)
In the Property Manager, pick the 2 faces that you want to set up as measurement faces. The measurement is the dimension that you are running the analysis for. In this case, it’s the distance between the front face of the bottom knife and the back face of the top knife. The nominal dimension is 0.1” and is highlighted in pink. SOLIDWORKS also gives us a green message letting us know the measurement is defined. Hit the blue arrow to the top right to go to the next step. Step 2 is telling TolAnalyst the order/sequence of how the assembly goes together. Mimicking the real world assembly sequence, it will be as follows: the lower knife block, the lower blade, the 2 guide pins, the 2 bushings, the upper knife block and finally, the upper knife. Just select the parts in the proper order, and you can right click on a part and delete it if it’s out of sequence. While you are selecting, the rest of the parts in the assembly remain transparent until they are selected. SOLIDWORKS also provides you with a “Neighbors” box which you can use to select parts next to the one you are selecting, or you can select them from the graphics area. Once you have selected everything, you get the nice green message. Hit the right blue arrow to go to the next step. Step 3 is defining the constraints in the assembly. TolAnalyst looks at the mates within the assembly for these constraints, which will define how the components are held together. Pick from all the available mates to specify primary, secondary and tertiary constraints depending on real world conditions. The first component is the lower knife block, which is fixed due to it being the first component in the sequence from the previous step, so we need to set up the constraints for the next component, which is the lower knife blade. You can see from the image, there are 2 mates to pick from, one on the bottom of the blade and one on the back of the blade: You can pick both of these constraints, but you really only need to constrain the blade in the X (red axis) direction, since the blade moving up and down in the Y direction won’t affect the tolerance stack up. If you hover over the flyouts, the faces that are being covered by that constraint highlight in green. Once you pick 1 or more constraints, the Component in the Property Manager has a green check next to it. Also, under that Components window, the Constraints window shows the primary, secondary and tertiary constraints and what faces they are between. After that, it’s just a matter of selecting the constraints for the other components. Click on the component, see what constraint or constraints pop up in the Graphics Area, and then select the number on the flyout. 1=primary, 2=secondary, and 3=tertiary. You can specify the constraint filters that you want to use, or just let SOLIDWORKS show all and pick from there. Everything in this assembly is pretty straight forward until you get to the Upper Knife Block. It has 6 possible constraints to choose from. This is where the green highlighting becomes key, so that we can pick the constraints between the OD of the bushing and the block (confirmed by the Constraints box). Just one last part to select, and that is the upper blade and its mount face. Next, I just have to hit the Next arrow again to run the study… and that’s where I’ll end this article (cliffhanger!)
Stay tuned for Part 3, and if you prefer, you can see my YouTube video here. Thanks for reading!