Join

One of the Join features is created in the active body. When this body is one half of a divided body that is in the document, then both the Join head and the Join thread features are created automatically. When instead the other half of the divided body is missing (either deleted or not created) or the active body is not the result of a division, then only the join head or thread is created. During the initial creation of the Join features, different non-active bodies may be specified as the body to connect the active one to.

Similarly to the Lip feature each of the two individual Join features has a separate life cycle. Therefore it is possible to delete the Join feature from each joined body separately.

This task shows you how to use the Join command to create Join features on associated bodies that were created by the same Divide.

1. Click the Join icon .
   The Join dialog box is displayed.

   By default during the creation of the Join, the Head and Thread buttons are selected. If the active body (in this case, Divide Body.3) is the result of a Divide and its associated non-active body (Divide Body.4) is present, the associated body is automatically selected as the entry in the Body to join field. Otherwise this field is blank. During the Join creation, this field can be cleared by clicking Head or Thread to deselect them. In this case, the Join feature will be a Head or Thread depending on which button is set; the associated Join Feature cannot be created afterwards. By selecting both Head and Thread options, the Body to join field is re-activated. And you may need to select a body in the Body to join field. Once you click OK, neither the Body to join field nor the Head and Thread options can be changed when editing them. When the Join is edited, the Body to join field will display the name of the associated body in gray color.

2. Select the point in the center of the plane (Sketch.2) as the Sketch for the Screw Positions.

   

   At each non-construction point defined in the sketch, a screw will be positioned. The tip of the arrow points to the body that will be the Thread. In this case, the lower body will have the Head geometry constructed within it. While the upper body will have the Thread geometry. By either clicking on the arrow or clicking on the Reverse Direction button, the tip of the arrow will be reversed, and therefore the geometries will be the opposite from what was described (i.e. the lower body contains the Thread geometry while the upper body contains the Head geometry).

3. In the Screw tab, check Countersunk head.

4. Define the parameters as shown below:

5. In the Head tab, the parameters as shown below:

6. In the Shank tab, the parameters as shown below:

7. In the Clamp tab, the parameters as shown below:

8. In the Thread tab, the parameters as shown below:

9. Now that the desired Join feature has been defined, click OK to create the feature.

In order to see better geometry view you just created, we will use the Divide feature to split the upper and lower bodies. The upper body is currently the active one so the Divide will modify it.

10. Click the Divide icon .

11. The Divide dialog box is displayed. The in-work body is detected: Divide Body.3 is to be divided. Select the YZ Plane as the dividing element. Uncheck Keep both sides checkbox. And then click the Reverse Direction button.

12. Click OK.

13. The lower body needs to be divided. Since the Divide feature works on the active body, it is necessary to make the lower body the active one by selecting Define in Work Object.

    Click the Divide icon .

14. The Divide dialog box is displayed. The in-work body is detected: Divide Body.4 is to be divided. Select the YZ Plane as the dividing element. Unselect Keep both sides checkbox. And then click the Reverse Direction button.

15. Click OK.

You can create a Join feature externally outside of the joining bodies. For the outside joins the Guide height should be set to 0.0. If the Guide height is not set to 0.0, the Guide will be added to the inside geometry but not the outside geometry. If Gussets are activated, they also only create inside geometry.

You can define gussets around the Head and the Thread of a join feature. A join feature often has stiffening gussets around the head, thread or both.

1. Click Join.1 under Divide Body.2 in the specification tree.

2. Select Gusset tab. Select Head in Gusset.

3. Uncheck Thread option in Join Features.

4. Enter the values as below.

5. Click OK to generate gussets.
   The geometry is produced for each of the points. Gussets are created only for the inside shapes. The geometry created for the outside point and outside portion of the boundary point do not have gussets.

You can select a screw from an existing screw catalog by clicking a screw catalog icon in Join dialog.

The selection of the screw will fill all the related parameters that affect the join design. A string attribute will hold the screw name and may be used to search for all Join features that use a particular screw from the catalog.
You can change the parameters related to the screw after you select from the screw catalog. If the parameters are changed, the display on screw tab goes back to “Custom Screw”.
 The join parameters in the form are updated with the values of the selected catalog screw. When the user modifies “Height” the screw reverts to “custom”. Final modified Join values = catalog values + modified value.