Have you used SOLIDWORKS Mate Controller? A part of the assembly mode, SOLIDWORKS 2016 added this function to allow you control over the movements of your assembly by adjusting some specific mates manually. You save positions in time and use them to make professional looking animations.
What You Need to Start
Let’s start with an assembly you have created. In order to use Mate Controller, the assembly must have these types of mates:
- Limit Angle
- Limit Distance
- Slot (Distance Along Slot, Percent Along Slot)
- Width (Dimension, Percent)
- Path (Distance Along Path, Percent Along path)
This Tiger I tank has various types of supported mates in it, so it will serve as an example.
How to Use Mate Controller
While in SOLIDWORKS’ assembly mode, go to Insert and select Mate Controller, the third option from the top. Depending on the version of SOLIDWORKS you are using, the menu should look something like this.
The symbol mimics a robot arm, which is a perfect example for mate controller. The menu has three sections: Mates, Mates Positions and Animation.
At first, the only active section is Mates and the others are grayed out. Click on the only button available. This button “collects all the supported mates” automatically. There are two possible outcomes: either SOLIDWORKS lists your supported mates in that blue field or you will get a warning that “there are no valid mates.”
Tip: Assign meaningful names to these specific mates so you won’t end up with a menu filled with Limit Angle1, Limit Distance 2.
Once SOLIDWORKS lists your mates in the field, you will see the second section, Mates Positions, as well as two up and down arrows in the first section. You may use the arrow keys to change the order of your mates in the first section. On the second section, you have seven buttons, two of which are grayed out:
- Add Position
- Update Position (originally grayed out)
- Reset Position (originally grayed out)
- Delete Position
- Reorder Position
- Make All Mates Driven
- Add Configurations
Now, all of the listed mates each have a variable value, a bar to adjust their value by dragging and a lock button.
Position 1 is now activated by default. Whatever change you apply to any or all of the mates (by dragging their bars), will be assigned to Position 1. For example, you can leave all the values like they are and change only the Cannon Rotation Angle from 30 degrees to 70 degrees. In order to save these settings, I have to click on Update Positions, which is no longer grayed out.
Add Positions and Update Positions
To adjust the setting for the second position, you may either change the values first and then click on Add Positions or first click on Add Positions and then change the values. Regardless of the method you chose, click on Update Positions to save it.
You will see the effect in the figure below with the Cannon Rotation Angle. Pay attention to the purple and orange highlights, which appear on the parts in the assembly, on which your mates are assigned.
Now I am going to do the following steps:
|Position||Name||Original Value||New Value|
|Position 2||Cannon angle 20||14 degrees||20 degrees|
|Position 3||Trap door closed||150.53 degrees||0 degrees|
|Position 4||Back hatch||0 degrees||55 degrees|
Reset, Delete and Reorder Positions
Now we have four positions saved. The next two buttons, Reset Position and Delete Position, are self-explanatory and intuitive. Reorder Position allows you to rename, reorder and delete your saved positions in its pop-up window.
Make All Mates Driven
This button may be the mother of all single “lock” buttons. In order to understand the function that this button carries in SOLIDWORKS, you need to understand what single lock buttons do. Once you enter the Mate Controller mode, you can no longer drag your parts manually. All changes have to be done through the mate controller menu—unless, you click on a specific mate’s lock button, then you unlock that part and allow it to be dragged freely by your mouse cursor. Of course, if you do drag that specific part, then the value in the mate controller’s menu will gray out and gets adjusted automatically.
If you would like to make different variations of your movements, use this button to save the combination of your saved movements under a new configuration. You can find them later in the Configurations Manager tab.
This is where the mates pay off. Open this option, and you will find all your saved positions listed in the right order in a table with a specific duration in seconds (usually 2 seconds on default). Of course, there are the typical SOLIDWORKS’ Play and Stop buttons on the bottom of this section. What you can do is to click on Calculation Animation—the calculator looking button with a small gear on it—to play your animation and see how you have done so far. If you would like to adjust a position’s speed, you can simply double click on its duration and change it.
You can also choose whether you would like to play all the positions or a specific range of your positions e.g. position 2 to 4 only. For that, SOLIDWORKS has covered you with a Select Positions option.
Once you are happy with the results, you can save your animation.
If you are keen to see the result of this very example, watch the video below.
About the Author
Ryan Fallahi has been working with SOLIDWORKS since 2007, as a mandatory module in mechanical engineering, but is hooked to this day. In addition to working with the software, he teaches beginners and intermediates the tips and tricks that took him years to learn by doing. This way, they can follow down a similar path but at greater speed and with higher quality by following his weekly blogs and tutorials at solidworkstutorials.net/blog.