 |
Frequently Asked Questions about Control Definitions
Q. What is a control definition?A. A control definition is a series of settings representing parameters for your machine’s control and your post processor. All of the numbered questions that were stored in the post processor in earlier versions of Mastercam are now set through the control definition in Mastercam X. In addition, each control definition is linked to a specific post processor and machine type.
Q. What does a control definition do for me?A. The control definition has two main functions. First, it provides Mastercam with information about the capabilities of your control. Second, it provides the post processor with information regarding your control and default post settings. Many settings that used to be stored in the post processor are now much more easily accessible in the control definition, reducing the chance that they will be overlooked or set incorrectly.
Q. How do I create a control definition?A. Use the Control Definition Manager (CDM) to create and edit control definitions.
Q. What is the Control Definition Manager?A. It is a graphical tool used for working with control definitions. The Control Definition Manager lets you set the product type, add a post processor, configure the control and post settings, and save your control definitions in .control files. The many different settings in a control definition are grouped into several different pages that are listed at the left side of the Control Definition Manager.
Q. It looks like there are several ways to start the Control Definition Manager. What’s the difference?A. You can start the Control Defintion Manager by either selecting it from the Settings menu, or by clicking a button inside the Machine Definition Manager. If you access it from the Machine Definition Manager, you can only create or edit control definitions of the same type as the machine. 
Two different ways to start the Control Definition Manager
Q. Where are the control definitions stored? What’s the file extension of a control definition?A. Control definitions are stored in .control files, in the CNC_MACHINES subfolder of your Mastercam installation folder. Each .control file can store several control definitions—just like in your shop, you can use the same control with different machines or post processors.
Q. Can you have more than one control definition stored in a .control file?A. Yes. The .control file is like a 3-ring binder. Each control definition is like a page in the binder. You can add or remove control definitions from the .control file just like adding or removing pages from a binder.
Q. If I can have multiple control definitions inside a single .control file, how does the Control Definition Manager manage them?A. Each control definition is tagged or defined by the product type and the post processor assigned to it. For example, if you have fanuc.pst, the same .control file can have separate control definitions for Mill-fanuc.pst, Lathe-fanuc.pst, Router-fanuc.pst, and so on. If you add a new post, you can then add another group of control definitions linked to it. This gives you a great deal of flexibility to manage control definitions and post processors in the way that makes the best sense for your shop. Large shops with many machines and controls can use control definitions to efficiently manage many post processors across many platforms, while a smaller shop might need only a single control definition in a single .control file.
Q. Can I mix control definitions for different products into one .control file?A. Yes.
Q. Do I have to have multiple control definitions in a .control file?A. No, you can have a single control definition in a .control file. In fact, many users will start out this way when they begin working with Mastercam X until they get more experienced with the control definition architecture.
Q. Is the post processor stored inside the control definition?A. A copy of the post processor is not stored inside the control definition. Only the post’s path and file name are stored in the control definition. The post must reside on the local Mastercam workstation (or on your local network, if you're using a NetHASP) in order to post.
Q. What do you mean by a “local copy” of the control definition?A. When you select a machine definition from the Machine type menu, Mastercam automatically creates a machine group and stores a copy of the machine and control definition in it. These are saved with your part file. It is very similar to the way that earlier versions of Mastercam stored a copy of the tool definition in your part file when you selected a tool for an operation. You can edit the local copy of the machine and control definitions from the Machine Group Properties for local, job-specific overrides.
Q. I’ve set up my machine and control definitions, and used the Control Definition Manager to enter all my control definition settings, post text, and miscellaneous values. Does this mean I no longer need to edit the .pst file like in earlier versions of Mastercam to create custom posts for individual machines?A. No. Properly defined machine and control definitions will make it easier to create and manage your post processors—and they can certainly be used to extend the usefullness of the many standard posts supplied with Mastercam—but they do not replace custom post writing. The processing logic and custom values inside many custom post processors are outside the scope of the control definition.
Q. How do I tell Mastercam what control definition is being used?A. This is done in the Machine Definition Manager. In the same way that you assemble a machine tool on your shop floor by attaching a control unit to the machine tool, when you are creating a machine definition, you select a .control file. Mastercam then displays a list of the post processors for which individual control definitions have been created for the type of machine you are defining, and you select one. For example, if you created a Mill machine definition, chose fanuc.control, and then selected the MPFAN post, what you essentially did was tell the machine definition to search the fanuc.control file for all the mill control definitions that are stored in it, and then selected the control definition that has the MPFAN post assigned to it. In the future, whenever you select this machine definition, Mastercam will automatically use the MILL/MPFAN control definition from the fanuc.control file.
Q. What control types are supported in the Control Definition Manager?A. Each control definition needs to be associated with one of the following types:
Wire EDM Machines and wirepaths are not yet available in Mastercam X. Mill/Turn definitions can be selected for either a Mill or Lathe machine.
Q. Is the Mastercam interface affected by the control definition?A. Yes, in two ways. First, since the control definition specifies the post processor, the Mastercam interface is modified by the post text and miscellaneous values stored in the specific post. Second, there are several settings in the control definition that enable/disable features on various dialog boxes.
Q. In the Control Definition Manager, there are Valid and Invalid posts. What makes a post valid or invalid?A. A valid post means that the post specified in the control definition exists and is in the expected location. When you are working in the Control Definition Manager, it looks like this:
An invalid post is one that was specified in the control definition but cannot be found on the hard drive. For example, the post may have been deleted, moved, or renamed, or might reside on a different workstation. When you are working in the Control Definition Manager, it looks like this:
It is also possible to create a control definition without selecting a post processor:
This lets the post developer create basic settings for, say, a Haas control without having to develop a machine-specific configuration or start with the system defaults that may not be close to what is normal for that control. If you try to actually post an operation with these settings, you will not be able to, but will be prompted to select a valid post. Read the online help in the Control Definition Manager to learn more about Mastercam organizes control definition defaults.
Q. Can incorrect data paths affect whether a post is valid or not?A. Yes, if the data paths are incorrect for the location of the post, the post will not be available and therefore be invalid.
Q. Can I store my posts in a network location?A. Mastercam's control definition architecture supports this if you are using a NetHASP. Use an absolute network location.
Q. The Communications button in the Post Processing dialog seems to be redundant. Those settings are already in the control definition. Are they likely to change for any particular operation?A. When you are communicating with the machine, it is important that you can override the settings if you want. This also lets you see what the settings are at the time of communication and helps as a development and troubleshooting tool. Also, if you are using a third-party communications package such as Cimco, the default settings are not stored in the control definition, so the Communications button gives you more flexibility for other communications options.
Q. Why can the operation defaults and operation libraries be set from the control definition?A. This lets you maintain sets of toolpath and operation defaults for specific controls or machines if you wish, as well as different sets of operation libraries. When you select different machines or controls, the different sets of defaults are also automatically selected. Note: You can override this on a job-specific basis by selecting a different set of defaults in the Machine Group Properties for an individual machine group. It is important to understand that the values for the operation defaults are stored separately from the control definition. Operation defaults are stored in a .defaults file. This lets you use the same set of defaults for all your controls and machines, if that is all you need. The Control Definition Manager just gives you a convenient way to access them.
Q. Why are these set in the control definition and not the machine definition?A. Generally, the control has more influence over the NC parameter information than the machine design. Tool settings are in the machine definition file using the same logic. However, if you want your operation defaults to be machine-specific, you can accomplish this easily by simply creating a different control definition linked to the different defaults.
Q. How does this work in conjunction with the .defaults file and .operations file that I choose in the System Configuration dialog box?A. The selections that you make in System Configuration are used when you create a new .control file. You can then select different files in the Control Definition Manager if you wish. The selections from the Control Definition Manager will be the ones that are actually used.
Q. Does that mean that I can have one .control file that uses two post processors, and each post can have a different set of toolpath defaults and operation libraries?A. Yes, the settings in each control definition category are specific to each post that is used in the .control file.
Q. Why does a green check mark appear over a control definition topic when I enter it?A. This indicates that you have viewed that page in the current Control Definition Manager session. That does not mean the the settings have been saved or are “correct.”
Q. Is this green check maintained after exiting the Control Definition Manager?A. No, when you enter a topic in the Control Definition Manager, the green check mark is applied to that topic. You will be asked to save those changes when you exit the Control Definition Manager.
Q. How are the post questions handled in X?A. There are no more post questions in X. All the settings that were accessed by numbered questions in earlier versions of Mastercam are now set in the control definition.
Q. On a CD data page, you can right-click and choose Default for either the current page or all pages. What default settings are you using – the default settings for that control type or the system defaults?A. You're referring to this menu, which is available on most pages in the Control Definition Manager. The default values can come from either of two places. In the post processor list in the Control Definition Manager, you can see an entry for “Default settings for control type.”
This is essentially a separate control definition that you can create and save in the .control file. If you have created and saved these settings, they are the default values that will be retrieved by this menu item. If these default values have not been saved in the .control file, Mastercam will reset to the system defaults.
Q. How do I use the Manufacturer and Description fields? Why are there two?A. The Manufacturer is a global string for the entire .control file. Change it anytime and it applies to all the control definitions in the file. The Description is specific to the current control definition. This way, you can have a one string for everything and one for each definition.
Q. In the Control Definition Manager, there are two options for rapid motion that seem to do the same thing—what is the difference between them?A. The options on these two pages both seem to do the same thing:
The first item is describing how you want the simulation (Backplot) to display the NCI motion. The second item is instructing the post to make the conversion for the NC output.
Q. Can I use the Control Definition Manager to create control definitions with my Version 9 post processor?A. Post processors from earlier versions of Mastercam are incompatible with Mastercam X and you cannot use them in control definitions. Use the UpdatePost utility to convert them, and then they can be selected and used to post toolpaths. Since the control definition includes so much information that used to be stored in the post processor, the UpdatePost utility can also create a control definition and machine definition based on information in your earlier post. For many users, this will be the easiest and fastest way to transfer settings from their current post processor to Mastercam X. UpdatePost is described extensively in the online help and in the Transition Guide.
Q. Why has the "Canned text" check box been removed from the Toolpath parameters page for all toolpath types?A. It is now part of the control definition. When a coolant type is set or canned text is set and used from the control definition, an asterisk is displayed on the appropriate button in the toolpath parameters, and can be viewed by selecting the button.
|
