If you create images or illustrations with Adobe or Microsoft products then you will be accustomed to grouping text and annotation elements together to make them easier to manage, move, or manipulate. Well when working with SOLIDWORKS Drawings you can use the same grouping elements technique with notes, dimensions, and other annotations. Although I have discovered a few limitations with the SOLIDWORKS Group command which I will point out in this tech tip.
To group elements together in your drawing simply select two or more annotations (either CTRL or window/box select) and then right-click and select Group > Group from the shortcut menu as shown below:
As with other applications the behaviour is the same for groups in SOLIDWORKS. For instance when entities are grouped together you can:
- Move one entity and the others in the group will move with it.
- Change the layer of an annotation in the group the other grouped entities will also change layer.
- Delete an annotation in the group and the entire group will be deleted.
You can add annotations to an existing group by selecting a group along with another annotation and pick the group command from the shortcut menu. But see the limitations below when trying to achieve this.
SOLIDWORKS Group command limitations
So there are limitations for the SOLIDWORKS Group command and when selecting multiple entities you may find that the group command is not available from the menu:
- Annotations must be related to the same drawing view. For instance when selecting dimensions that are assigned to different drawing views the group command may not be available.
- Blocks can be grouped. The group command is available when selecting blocks, however groups that contain blocks will not act like other groups e.g. a block will not move with the group.
- Moving a group and then using undo does not move the entire group back to its original position. This is annoying when dragging annotations it moves the entire group, but if you select undo only the selected annotation returns to the original position?!
- It’s hard to tell what is in a group. When selecting some entities black control points will appear on other entities in the group, but this doesn’t apply to all annotation types.
- You can’t group multiple groups together. Again this is another annoyance as grouping groups together is really handy in other applications. See the error message in the image below:
Moving entities independently of the group
Just like other applications you can move an item independently of the SOLIDWORKS group if required, there are a couple of methods to achieve this:
- Hold down the ALT key when dragging an annotation and it will move independently of the group
- Or pick an internal control point of an annotation and drag, it will move independently of the group
You can ungroup the entire group or remove an annotation from a group as described below:
- Ungroup an entire group by right-clicking an annotation in the group and select Group > Ungroup
- Right-clicking an annotation you want to remove from a group and select Group > Remove From Groups
To learn more about working with annotations you should attend a SOLIDWORKS Drawings training course either live online or in a classroom near you
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