PartDesign MultiTransform

Description
The PartDesign MultiTransform tool creates a pattern of one or more features. The pattern can include multiple transformations where each subsequent transformation is applied to the result of the previous transformation.

The available transformations are: Mirrored,  LinearPattern,  PolarPattern and  Scaled. The first three are also available as separate tools.



Create

 * 1) Optionally activate the correct Body.
 * 2) Optionally select one or more features in the Tree view or the 3D view.
 * 3) There are several ways to invoke the tool:
 * 4) * Press the button.
 * 5) * Select the option from the menu.
 * 6) If there is no active Body, and there are two or more Bodies in the document, the  dialog will open and prompt you to activate one. If there is a single Body it will be activated automatically.
 * 7) If no features were selected the  task panel opens: select one or more (hold down the  key) from the list and press the  button.
 * 8) The  task panel opens. See Options for more information.
 * 9) Press the  button at the top to finish.

Edit

 * 1) Do one of the following:
 * 2) * Double-click the MultiTransform object in the Tree view.
 * 3) * Right-click the MultiTransform object in the Tree view and select from the context menu.
 * 4) The  task panel opens. See Options for more information.
 * 5) Press the  button at the top to finish.

Combine existing transformations
It is possible to create a MultiTransform object from existing Mirrored, LinearPattern and PolarPattern transformations.


 * 1) Check the  property of the existing transformations to make sure they have been applied to the same features.
 * 2) Select those features in the Tree view.
 * 3) There are several ways to invoke the tool:
 * 4) * Press the button.
 * 5) * Select the option from the menu.
 * 6) The  task panel opens.
 * 7) Press the  button at the top.
 * 8) Edit the  property of the created MultiTransform object:
 * 9) Click in the field.
 * 10) Press the  button that appears.
 * 11) The  dialog opens.
 * 12) Hold down the  key and select the existing transformations.
 * 13) Press the  button.
 * 14) Optionally edit the MultiTransform object, see above.

Options

 * To add features:
 * Press the button.
 * Select a feature in the Tree view or the 3D view.
 * Repeat to add more features.
 * To remove features:
 * Press the button.
 * Do one of the following:
 * Select a feature in the Tree view or the 3D view.
 * Select a feature in the list at the top and press the key.
 * Right-click a feature in the list at the top and select from the context menu.
 * Repeat to remove more features.
 * If there are several features in the pattern, their order can be important. See PartDesign PolarPattern.
 * To add transformations:
 * If there are existing transformations: select the transformation after which the new transformation should be added.
 * Right-click the list.
 * Select one the following options from the context menu:
 * . See PartDesign Mirrored.
 * . See PartDesign LinearPattern.
 * See PartDesign PolarPattern.
 * . See PartDesign Scaled.
 * The selected transformation is added to the list and the settings for the transformation are displayed below the list.
 * Adjust the settings to suit.
 * Press the bar at the bottom.
 * Repeat to add more transformations.
 * To edit a transformation:
 * Right-click the transformation in the list.
 * Select from the context menu.
 * Adjust the settings to suit.
 * Press the bar at the bottom.
 * To change the order of the transformations:
 * Right-click a transformation in the list.
 * Select or  from the context menu.
 * If the checkbox is checked the view will update in real time.

Limitations
See PartDesign PolarPattern.

Example
You can use this function to create a fully parametric part that is symmetrical about two axis from a sketch. This could be a 150x100x10mm large mounting plate for a stepper motor with symmetric holes and a pocket.
 * create a "quarter" part from a sketch that covers the first quadrant of the part (i.e. upper left quadrant in Sketcher).
 * note that your constraints must only cover a quarter of the part. You can use use construction geometry with the full part dimensions are constrain against those or just use halved values for X and Y sizes, e.g. instead of a full dimension of 150mm enter "150/2mm" or "75mm"
 * Make sure the sketch is closed by adding lines along the vertical and horizontal axes to the origin.
 * close the sketcher and extrude the part with PartDesign Pad.
 * Select MultiTransform
 * a task dialog will open. As default feature the last tip from the tree is aleady listed. Since we want to mirror the complete part we do not need to any any feature.
 * click with the right mouse button into the "Transformations" field and select add mirrored transform
 * Select under "Plane" the correct axis: Vertical sketch axis
 * now you should see you part mirrored about one axis
 * click again with the right mouse button into the "Transformations" field and again select add mirrored transform
 * Now select under "Plane" the other axis: Horizontal sketch axis
 * note: if you forget to select the other axis the part will be mirrored twice along the same axis. Visually nothing will change but you have twice the goemetry.

Now you part is mirrored about the two sketch axes. You can edit the transforms any time by double clicking the "MultiTransform" icon in the tree.

To verify that the part is fully parametric open the initial sketch with the quarter part and change one dimension, say a hole position. After closing the sketch all 4 holed will have changed accordingly. This works with all other dimensions as well. Compareed with a sketch modelling the full part with a signle extrusion but no mirroring, the skeck would be a lot more complex with a lot of redundant information. All later changes would be more complicated. This sketch is small and easy to change.