This chapter is from the book
This chapter is from the book
This chapter is from the book
4.6 Macros
Design automation offers two benefits. First, it enhances productivity. Second, it helps with repetitive tasks that are mundane. For example, if you follow the same design process over and over, automating it would be the logical thing to do.
Macros aid in design automation. Macros are also viewed as a way to customize your CAD/CAM system. A macro is a short computer program that is used to repeat commonly performed operations. That computer program is generated automatically by a CAD/CAM system in the background during use of the system, from the time you turn on the macro until you turn it off. You can use the macro after creation over and over, with different input values (e.g., new dimensions). After you create a macro, you can use it for recording, edit it, run it, pause it, stop it, and assign it to a shortcut key (hotkey) or to a menu item. When you assign a macro to a shortcut key or to a menu item, you can specify which method (function) of the macro to run. Click Tools > Macro to access the macro menu. SolidWorks saves the macro file in the same part folder and uses .swp as the file extension, with the default names Macro1.swp, Macro2.swp, and so on, unless you change them.
A higher level of automation than using macros is to use Visual Basic (VB) or another programming language to perform full automation and have better control of the automation. As a matter of fact, VB is the programming engine behind macros. Instead of writing the macro VB code, the SolidWorks macro interface enables us to generate the code automatically while you perform the design tasks as usual. It is this VB code that you save in a file when you save the macro. You can use the VB editor to edit and tweak the VB code.
Macro VB code uses the SolidWorks API (application programming interface). The code makes calls to API functions. Think of the API as a gateway between the application you want to write and SolidWorks code that has been already written. In other words, the API provides access to the SolidWorks geometric engine.
You can learn VB programming by creating multiple macros, studying their generated VB code, and expanding on it. VB is an object-oriented programming (OOP) language that requires knowledge and understanding of object-oriented design and how objects are defined and implemented.
The programming approach could be useful for creating an entire assembly from a few parameters. You can write a program to define some variables and store them in a row in a design table. Each row represents a new version of the assembly. You delete all rows from the table and keep the last row, which is the new assembly.
Example 4.4
Develop a macro to create an extrusion.
Solution This example illustrates the creation and use of macros. It shows how to create a block extrusion and record the steps of creating it in a macro.
Step 1. Turn on macro and create Sketch1 and Boss-Extrude1 feature: File > New > Part > OK > Tools > Macro > Record > Front Plane > Extruded Boss/Base on Features tab > Sketch tab > Center Rectangle on Sketch tab > sketch a rectangle and dimension as shown > exit sketch > enter 2 for D1 > reverse extrusion direction > ✓ > File > Save As > example4.4 > Save.
Note: Macro > Record opens the Macro recording window shown. Hover over its buttons to read them.
Step 2. Stop and save macro: Tools > Macro > Stop (or click black square on Macro window shown in Step 1) > type BlockShaft for macro name in the Save As window that opens > Save.
Note: The full macro file name is BlockShaft.swp. The default folder for the file is the part file folder from Step 1.
Step 3. View the macro VB code: Tools > Macro > Edit > select BlockShaft.swp > Open. The editor displays all the lines of code associated with the macro. Figure 4.9 shows the first lines of the macro VB code. Explore the code and try to understand which sections pertain to which steps performed in SolidWorks.
Step 4. Run the macro: Open a new part or delete the feature from the current part > Tools > Macro > Run > select BlockShaft.swp > Open > enter 8 for rectangle width when dimension box appears > ✓ > enter 6 for rectangle height when dimension box appears > ✓.
)
Figure 4.9 VB editor window
Example 4.5
Create a hotkey for a macro.
Solution This example assigns the macro from Example 4.4 to the Shift+X hotkey on the keyboard. When the user presses this combination on the keyboard, the macro runs.
Step 1. Create macro hotkey: File > Open > locate example4.4 > Open.
Step 2. Locate macro file: Tools > Customize > Keyboard tab > scroll to bottom and locate Macros row > click ellipsis button (...) in this row to open window shown > click the browse button (...) > locate macro file (.swp extension) > Open > OK.
Step 3. Create hotkey: Click Shortcut(s) column in Macros row as shown > Shift+X to add shortcut as shown below > OK.
Step 4. Use hotkey to run macro: Press Shift+X in an open part.