Place Tangent constraints in assemblies

Use the Constrain command or Assemble command to place a Tangent constraint between assembly components. A Tangent constraint positions faces, planes, cylinders, spheres, cones, and ruled splines tangent to one another.

To begin, place the components to constrain in an assembly file.

Use Constrain to place Tangent constraints

On the ribbon, click Assemble tab Relationships panel Constrain .

In the dialog box, under Type, click Tangent. Select the first face, curve, or work plane. If necessary, click First Selection to enable the selection. Use Select Other to cycle through geometry. Select the second face, curve, or work plane. If necessary, click Second Selection to enable the selection. Use Select Other to cycle through geometry. Enter an offset value, if applicable. Click Inside or Outside to specify the tangency position. Click the More button to change the name the constraint or set limits. In the Name box, enter a constraint name, or leave blank and a default name is automatically created. Check Maximum and enter a value to specify the maximum limit position. Check Minimum and enter a value to specify the minimum limit position. Check Use Offset As Resting Position and enter the required value in the Offset value box to specify the resting position. Clear the check box to remove limits. Values are retained in an inactive state. If Show Preview is selected, observe the effects of the applied constraint. If either component is adaptive, constraints are not previewed. Click Apply to continue to place constraints or click OK to create the constraint and close the dialog box. Show Me how to create a tangent constraint

Use Assemble to place Tangent constraints

On the ribbon, click Assemble tab Relationships panel Assemble .

Select a face, curve, or work plane on the component that changes position. Select a face, curve, or work plane on the component remains in position. Enter an offset value, if applicable. Change the solution from Outside to Inside to specify the tangency position. Do one of the following: Click Apply and continue to define constraints. Click OK to create the constraint and exit the Assemble command. Click Undo to delete the selections and continue to define constraints.

Note: If other components obscure selection, do one of the following:

• Temporarily turn off visibility before you place a constraint. Click to select a component, right-click, and then select Visibility.
• To restrict selectable geometry to a specific part, select Pick Part First in the dialog box, and then click the component you want to constrain. Clear the check box to restore the selection mode.