Sketch Entities and Mates

Article by Joe Medeiros, CSWE created/updated September 14, 2013

Note: The information contained in this article applies to SolidWorks 2013 and earlier versions. Next week we will show you how an extremely powerful new tool introduced by SolidWorks 2014 empowers users to replace sketch entities without breaking relations downstream.

After opening an assembly, mate errors are present, that were not present when the assembly was last saved.

mate errors

On troubleshooting the mate errors, it is evident that a mating face is missing.

missing face

Often the reason for the mate error is due to a sketch entity being deleted and possibly replaced. When a sketch is used to create an extrusion, each sketch entity will generate a face and this face will have a unique ID. If a sketch entity is deleted and replaced with another sketch entity, this will result in a new face with a new unique ID. In an assembly, mating faces are identified by this unique ID. If a change in a sketch results in a new face with a new ID, then this may result in mate errors if the old face face was referenced in a mate.

To avoid these errors, avoid deleting sketch entities when possible. If this is not possible and you believe that the changes may affect some mates, open the assembly and fix the mate errors. Mate errors can be difficult to troubleshoot; fixing them as they occur will make fixing them much easier. Some people avoid mating to faces altogether and instead mate to planes. Care should be taken not to reference a model face when creating a plane, as model changes may cause rebuild errors on the plane. If the assembly does not have any moving parts, using the mate option Use for positioning only may prevent mate errors even if the sketch geometry is changed.

mate options

This option will position the component, but will not apply any mates. When the component is correctly positioned using whatever “position mates” that are required, the component can be Fixed. This method would also increase performance, since there are no mates to process during rebuilds.

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Joe Medeiros, CSWE

Joe Medeiros is a SOLIDWORKS and PDM Certified Expert. He has been helping SOLIDWORKS users with training, mentoring and implementations since 1998. He combines industry experience with a thorough understanding of SOLIDWORKS products to assist customers in being successful. He shares his experience and expertise through blogs; one of which has been incorporated into the SOLIDWORKS Essentials training manual.