Using Angle Limit Mates to Replicate Collision Detection in Assemblies

One of the biggest benefits of having an assembly built in SOLIDWORKS is that it gives you the best digital representation of the physical end product. You’re able to verify part fitment, run complex simulations, or even create detailed documentation packages.

The easiest way to get a one-to-one representation of the real world is to restrict your assembly’s movement based on collisions between components. Fortunately, you can utilize angle limit mates to replicate collisions and enhance your SOLIDWORKS assemblies. We’ll walk through the steps to create a mate that will stop the collision of objects when they collide.

The Move Component Command

Activate the move component tool from the Assembly tab of the Command Manager. Once we have this tool active, we can then perform a collision detection to determine our angles. In the Move Component command, you can select Collision Detection and then specify the collision between two components.

In my case, I am doing the check between the Base Plate part and the Pipe part. After selecting those two components, I will click on Resume dragging until the two items collide.

Create the Angle Mate

Start by opening the Mate command and selecting the two reference planes from the flyout Feature Manager. In this specific assembly, I want to find the angle between the Top plane of the Pipe and the top plane of the Base Plate, so I will use this angle to create an angle mate.

Creating the first part of the assembly mates

By default, the two planes may become parallel once you start the mate, but selecting angle mate will return it to the proper angle. Check off the box, and the first part of our job is complete. The pipe is in a defined position pressing against the knobs of the base plate.

Suppress the Mate to Measure the Second Angle

After we create the angle mate, we will then have to suppress it in order to create the second part of it. After suppressing, we can run the collision detection, but this time, rotating the pipe to the lower knob. If we were to create a second angle mate in this position, it would cause errors with the first one we created.

Measuring the angle where collision occurs

Instead, we will take the Measure command from the Evaluate tab of the Command Manager to find the current angle between the two reference planes from earlier. In this instance, the current angle is 27.31 degrees.

Using Angle Limit Mates to Represent Collision

At this point, we can unsuppress the angle mate created earlier. By editing that mate and changing it to an Advanced Angle mate, we can supply a range of angles that the component will stay between. The first angle should be automatically set from the original mate, and the second one can be input from the measurement taken above. By setting the angles accordingly, the rod will only be able to rotate between the two knobs and will accurately represent real-world collisions.

Creating the angle limit mate

To learn more powerful modeling and mating techniques, register for an upcoming SOLIDWORKS Assembly Modeling training course here.