Unless you are completely new to SolidWorks, you have more then likely used the Coincident mate. It is probably the most common mate used when building assemblies. Today, we are going to look more into using the coincident mate to limit the degrees of freedom in your assemblies. If you are familiar with the Coincident mate, stick around… I am going to discuss another approach to adding the mate you might not of heard of before.

The Coincident Mate

One of the hardest parts about writing articles about SolidWorks is coming up with models that would best illustrate the points. After many failed attempts, I finally settled on using a model of a brick wall to show how the Coincident mate can be used. In the following steps, I will be showing you a couple of different ways you can apply the coincident mate to a brick to define its location on the wall. The use of the coincident mate will come pretty close to how mortar would be used on a real brick wall except for some minor differences. 

If you are not familiar with the Coincident mate, it is used to ensure that two planes, faces, edges or points (or any combination of these types) are in constant contact between two components. In all cases, just one mate will not be sufficient to limit the degrees of freedom for the part. For example, in our brick wall example if we just added a Coincident mate between to faces of two bricks. The part can still be moved in the assembly as long as the two selected faces share the same plane. The faces do not even need to touch. I think it will all make more sense when you see the example, so let us go ahead and jump right into it.

Adding The Coincident Mate

After inserting a component into an assembly, you will see in the FeatureManager that its location is under defined with the minus (-) that is shown next to the model name. We will need to limit the part Degrees of Freedom before the symbol is removed.

1.   Click S on your keyboard and select Mates from the Shortcut Toolbar.

2.   Select the front face of the brick by clicking and releasing the left mouse button.

3.  Select that face on the select part that will be mated. This part should, in most cases depending on your design, already have its position fully defined.

Mate Pop-up Toolbar

After releasing the left mouse button after selecting the second part, a Mate Pop-up Toolbar will be shown near the mouse pointer. The mate that is most appropriate based on the selections made in the Graphics Area will already be selected in the toolbar. If you need to select a different mate, you can make that selection in the toolbar rather then the Mate PropertyManager. If no other options need to be set, clicking the green checkmark in the toolbar would apply the mate and allow you to move onto another selection.

Mate PropertyManager

There maybe times when you need to set options that affect how your mate acts.In addition to setting options for the selected mate, you can also change the mate type in the Mate PropertyManager. Honestly, out of habit, I will confirm my mate selections in the PropertyManager instead of the Mate Pop-up Toolbar but this is something I am trying to address. 

Mate Alignment

Near the bottom of the Standard Mates section in the Mate PropertyManager, the alignment of the mate can be adjusted with two buttons. The first button, Aligned, is usually the default when using a Coincident mate but it depends on the selection and the orientation of the parts prior to mating.

Aligned

The Aligned option orientates the moveable component so that both of the selected faces are pointing in the same direction.

The view below shows how the two selected faces are pointing in the same direction when the Aligned option is selected in the Mate PropertyManager.

Anti-Aligned

The Anti-Aligned options orients the moveable part so that the two selected faces are facing each other.

The view below shows how the brick is rotated to have the selected faces opposing each other when the Anti-Align option is selected in the Mate PropertyManager.

 After selecting the appropriate faces, edges, points or planes and the options have been set in the PropertyManager, clicking the green checkmark in the PropertyManager will apply the mate and you can move on to the next mate. If you are done applying mates, clicking the green checkmark or hitting ESC will exit the Mate PropertyManager.

Using SmartMates

As promised, here is a great way to apply mates that you might not have head about before. SmartMates are used to apply the most commonly used mates without the need of the Mate PropertyManager. Throughout future posts, we will explore SmartMates with different mate types but today lets just look at how the Coincident mate can be quickly and easily applied.

1.  Instead of initiating the mate command, if you hold the ALT key and select the desired face of the part and drag the part to to the target part. The mouse pointer will update to include a small paper clip icon.

NOTE: If you hold the CTRL key instead of the ALT key, the part will be copied and used to mate to the target part. 

2.  When the mouse pointer is directly over another surface, the mouse pointer will update to include a symbol describing the type of mate being applied. In this case, the pointer shows that two planar faces are being mated.

Changing the Alignment when Using SmartMates

Even though the Mate PropertyManager is not being used with SmartMates, the alignment can still be specified. While still holding down the left mouse button, release the ALT key and press the TAB key to flip between the two aligment options.

Accepting the Mate

 To accept the mate, first release the left mouse button and then click the green checkmark in the Mate Pop-up Toolbar. Once the mate is applied, there is no need to close out of anything unlike when using the Mate PropertyManager. You can move on to another operation in your assembly or you can apply another mate using SmartMates. This is the reason why I prefer using SmartMates whenever possible.

NOTE: Even though they are not considered mates that are applied using SmartMates, you can change your mate type to any of the ones shown in the toolbar and still have no need to use the Mate PropertyManager.

Conclusion…

Once you finished defining the position of the part in your assembly, the minus (-) in the FeatureManager is no longer present. The part cannot be moved unless you delete the mates applied….but is a different post altogether.

I hope that even the more experienced SolidWorks users found today’s post helpful. Next time we will be going over the Parallel Mate, so keep on the look out for that one. Hopefully, it will be be posted soon. I promise

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