Apply Method

This command allows to apply a method into a document.

A method document defines a sequence of multiple commands to automate modeling tasks, resulting in significant time savings for repetitive modeling processes.

Creation stages / Use:

Select the Tools > Apply Method... command from the drop-down menu.

Select the method to apply.
Fill driver(s).
Validate.

The available methods are those present in the current project as well as those existing in its references.
No preview will be displayed when using a method.

Click on the following link to learn about the steps for creating a Method.

Handling of invalidities:

If, during the use of a method, an operation fails (because it cannot be constructed), an assistant—made up of two icons located at the top right of the graphics area—allows you to correct the invalidity and then continue applying the method in order to create the missing operations.

First, if applying a method triggers an invalidity, TopSolid displays an error message indicating the invalid operation. When you validate this message, a second message appears to inform you of the procedure to follow:

Repair the invalidity.
Then use the command Resume Method Application…, available in the graphics area.

Quit Method Application: Allows you to exit the method application assistant. The method stops and keeps the operations that have been created (including the invalid operation). For example, if the invalidity occurs at the end of the method application, and depending on the complexity of the operations, it may be faster to manually rebuild the missing operations rather than correct the error and resume applying the method.

Resume Method Application: Allows you to resume applying the method after repairing the invalidity. This icon is only available once the error has been repaired. The method then builds the missing operations.

Activating the Resume Method Application… button allows you to continue creating the method operations. If a new operation triggers another invalidity, the process is repeated so that you can correct this second invalidity, but without displaying the warning message.
As long as the invalidity management assistant is active, it is not possible to apply another method. An information message is then displayed, asking whether you want to start a new application or not.
If an invalidity occurs while applying a method when the dialog was pinned, it is not possible to return to the method application dialog after the repair.

To correct an invalidity, you must edit the operation that is in error and repair it. You cannot delete it to create a new one, because in that case the method application assistant cannot be resumed. An error message will be displayed to inform you of this. If necessary, you can create new operations below the invalid one to help you repair it.

Example of repairing an invalidity:

Consider a part document containing a rectangular sketch from which an extruded shape has been created. On this shape, a constrained frame is added in order to drill the shape.
A method document is associated with this part. The sketch is dragged into the drivers. The operations folder then contains the extruded shape, the constrained frame, and the drilling operation.
In a new part document, a non-rectangular sketch is created.
The method is applied, the non-rectangular sketch is selected, and the dialog is validated. A first error message appears concerning the constrained frame; the operation is invalid. After validating this message, a second message appears, informing you to repair the invalidity and then use the Resume Method Application… button (unless you have chosen not to display this message again).
It can then be observed that the extruded shape has been created, but that the constrained frame is indeed invalid.
Edit the Constrained Frame operation to define the planes or axes that were not automatically found, and validate.
The document is no longer in error, but the drilling operation does not appear.
Select the Resume Method Application… icon; the method then continues and the drilling operation is created.

Case of an invalidity when applying a method containing a local extruded bar creation operation.
If the extruded bar operation is in error, after repairing it the extruded bar may be displayed as unbounded (length of 100 000 mm). This situation is normal: activating the Resume Method Application… icon completes the extruded bar creation process, and it will then be trimmed correctly.