Blog SOLIDWORKS Assembly Validation Tools – Part 1 - Move Component
This month, we are going to take a deep dive into SOLIDWORKS assembly validation tools. These tools are part of the standard SOLIDWORKS tools, most of which can be found on the Evaluate toolbar. The 4 main tools that we want to focus on in this series are: Interference Detection, Clearance Verification, Hole Alignment, and Move Component (found on the Assembly tool bar).
When we talk about assembly validation tools, we are not referring to SOLIDWORKS Simulation tools to run FEA (Finite Element Analysis) studies. These tools are used to assure that we have proper models before running FEA studies or releasing these parts to a manufacturing production environment.
Move Component
The Move Component command is found on the Assembly toolbar, or can be found under the Tools pull-down menu under Tools, Component, Move. When you select this option, you will notice that your cursor will change to, and you should see the Move Component property manager.
Under the Move settings, the pull-down menu has the following choices: Free Drag, Along Assembly XYZ, Along Entity, By Delta XYZ, To XYZ Position.
Free Drag – allows you to select any component and move it in any direction.
Along Assembly XYZ – allows you to select any component and drag it in the X, Y, or Z direction or the assembly. A coordinate system will appear on your model to help you orientate the direction.
Along Entity – allows you to select a reference component, then click and drag another component based on the reference component. If your reference is an edge you will have one degree of freedom; if your reference is a plane then you will have two degrees of freedom.
By Delta XYZ – allows you to type an X, Y, or Z value in the property manager and click apply. The component will move by the amount specified.
To XYZ Position – Allows you to select a reference point on a component, then type in an X, Y, Z coordinate in the property manager and click apply. The selected reference point of the component will move to that location. If you select a reference other than a point or a vertex, then it will place the parts origin at that location.
Under the Rotate settings, the pull-down menu has the following choices: Free Drag, About Entity, By Delta XYZ.
Free Drag – allows you to select any component and move it in any direction.
About Entity – allows you to select a line, an edge, or an axis, and then drag a component around the selected entity.
By Delta XYZ – allows you to type in an X, Y, Z value in the property manager and click apply. The component will rotate around the assemblies axis by the angular value specified.
The Options settings allow you to select what type of Move function you would like to perform.
Standard Drag – allows you to move a component from one position to another in an assembly.
Collision Detection – allows you to determine if one or more components will collide (prevent proper movement) when moved or rotated.
Physical Dynamics – allows you to move a component in an assembly and transfer forces from the moving component to additional components in the assembly allowing them to move based on their constraints.
The Dynamic Clearance setting will allow you to detect the minimum clearance between two moving or rotating components. A dimension will appear indicating the minimum distance.
Stop at Specified Clearance – Allows a user to specify a specific distance to stop at
The Advanced Options settings allow you to select additional functions you would like to occur
Highlight Faces – this will highlight the faces of the parts that interfere.
Sound – This will play an audible sound when the moving geometry interferes.
Ignore Complex Geometry – This simplifies the type of geometry that can be used for a collision detection. SOLIDWORKS will only use the following surface types: planar, cylindrical, conical, spherical, and toridal.
This Configuration – This only applies to Move Component or Rotate Component. This check box does not apply to Collision Detection, Physical Dynamics, or Dynamic clearance.
We hope this has given you a better understanding of the capability available in the Move Component command. Please check back for the rest of the series as we continue to take a deep dive into the SOLIDWORKS assembly validation tools that are available and how they work. Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SOLIDWORKS tools. All of these articles will be stored in the category of Daily Dose…..of SOLIDWORKS Support and links to each article with their release date are listed below: