 |
Frequently Asked Questions about Machine Definitions
Q. Why do I need Machine Definition in Mastercam? We have always been successful without it.A. The machine tool market and manufacturing industry are changing to combine many different processes within one enclosure. CAM software will need to have a complete definition of the machining environment to create accurate toolpaths for the new machine tool designs. Selecting a machine is a natural evolution from simply selecting a tool, like in previous versions of Mastercam, and it gives you correspondingly greater control over organizing your parts and machining jobs.
Q. What is a machine definition?A. A machine definition is a collection of settings that lets you model your machine, its components and peripherals, and its control—for example, a 5-axis machining center with a Heidenhein control; a lathe with two spindles and four turrets, and a Fanuc control; or a 3-axis HMC with a Fadal control. Mastercam customizes its interface based on your CNC machine. This means that Mastercam is aware of what the machine can and cannot do. Because of this, you are much less likely to enter incorrect information when programming in Mastercam, resulting in correct G-code output. Mastercam also uses the machine definition to determine which Mastercam product is running. For example, when you select a lathe machine from the Machine type menu, Mastercam automatically starts Mastercam Lathe. When you select a mill, you see Mastercam Mill functions and toolpaths.
Q. How do I get started creating a machine definition?A. Mastercam X installs many generic machines definitions representing common mills, lathes, and routers—for example, a 2-spindle 4-turret lathe, or a 4-axis HMC mill, or a gantry router. One approach is to start with one of these generic machines and customize it to match your specific machine. This could involve editing the parameters of the standard components, and then adding your own components—for example, a rotary table. Many users who are upgrading from earlier versions of Mastercam will use the UpdatePost utility to create a generic machine definition and control definition based on their current post processor. The new machine and control definitions will be linked to the updated post processor to get you up and running as quickly as possible. You can then customize the definitions as you wish. The Transition Guide that comes with Mastercam X, as well as the online help, contains a great deal more information about this.
Q. What’s the difference between a machine definition and control definition? How do they relate to each other?A. A machine definition is linked to a control definition, but they are separate groups of settings saved in separate types of files. Just like when you build an actual machine tool and bolt a control unit onto it, when you are creating a machine definition, you select a control definition file that will be used whenever you select the machine. By saving them in separate files, you can use the same control file with several different machines, and have a great deal more flexibility in organizing your work.
Q. How does the machine definition relate to the post processor? What if I need to use a different post with the same machine?A. Just like every CNC machine tool must have a control unit connected to it, every machine definition must be linked to a control definition. Each control definition is associated with a specific post processor, so when you are building the machine definition, selecting the control definition is basically the same thing as selecting the post processor. To select a different post processor, do either of these two tasks:
Using the machine group properties to select a different post processor. In either case, the only post processors that will be available to be selected will be those for which a valid control definition has been created and saved in the .control file.
Q. How will the Machine Definition Manager work with Wire? I want to be sure that X Wire will just be as functional as Mill, Lathe, and Router.A. It will work in the same fashion as Mill, Lathe, and Router, but with Wire-specific components and properties. The control definition will also be wire control specific for a future release.
Q. Is the Mastercam interface affected by the machine definition?A. Yes. For instance, if your machine definition has a maximum spindle speed of 10000 RPM defined, Mastercam won’t allow a value greater than 10000 to be entered into the toolpath parameters. If you are working with a 3-axis mill, for example, you will not be able to create a 5-axis toolpath. This minimizes the chance of entering incorrect information that would lead to bad G-code. Also, Mastercam uses the machine definition to determine which Mastercam product is running. For example, when you select a lathe machine from the Machine type menu, Mastercam automatically starts Mastercam Lathe. When you select a mill, you see Mastercam Mill functions and toolpaths.
Q. Do I have to have a machine defined and loaded to create toolpaths?A. Yes. However, it does not necessarily have to be your exact machine. We ship Mastercam with many standard machine types that can be used to program your parts. For example, you can select a generic 3-axis mill or 5-axis VMC. But for the best interaction with the least room for error, your machine and control definition should be customized to match your specific machine and control.
Q. What if I program a part for a specific machine and then decide to change to a different machine?A. Mastercam will validate your operations against the new machine definition and report on the compatibility between them. There are 3 basic levels of compatibility that Mastercam will identify for each toolpath:
Q. Can I have a Lathe, Router and a Mill machine definition in the same file?A. Yes. Because of Machine Definition, you can program for multiple styles of machines in the same file. For instance, if a part requires Milling, Turning and Routing operations, the part can be programmed in full, using 3 different machine definitions, and saved in a single MCX file.
Q. How do you keep track of all the machine definitions if you use multiple machines in a single file?A. Every time a new machine is loaded, Mastercam will create a separate machine group in the Toolpath Manager. All toolpaths created for a specific machine need to be located in that machine’s group. When you move from one machine group to another, Mastercam will automatically load the correct machine and change the interface to accommodate the current machine. For instance, if you change from a Lathe to a Mill, your toolpath selections will change from Lathe toolpaths to Mill toolpaths.
Q. If I already have a group of toolpaths and I need to change the machine, how do I do it?A. In the Toolpath Manager, click on the Files icon in the properties for that group, and choose your new machine by clicking the Replace button. 
Q. Will the Version 9 tool insert and holder catalogs (for example, Kennametal) be usable in X?A. Yes, they have been updated to work in X.
Q. Will the insert and holder catalogues be updated for X?A. Yes, the existing information has been updated to reflect current technology.
Q. Can I use my custom tool or holder catalogues that I created for Version 9 in X?A. To update a custom catalog you created in Version 9, you need to select the catalog using the Select Catalog button on the Insert tab of the Define Tools dialog box. The files will then be updated automatically when you open the Define Tools dialog box.
Selecting an insert catalog
Q. What does the Apply to all linear axes option on the Feed Rate Limits tab of the General Machine Parameters dialog box do or affect?A. This lets you set a global traverse rate that applies to all the linear axes without having to set it in each page.
Linear axis feed rate limits
Q. How are component libraries stored in Mastercam machine definition files?A. Component libraries are treated and saved as a machine type, just like a Mill, Lathe or Router machine definition file. If you are working on a component library, the machine type is “component library.” Use the File Open, Save, and Save As buttons to work with component libraries just like a regular machine definition.
Q. Why are there two sets of feed rate limits in the General Machining Parameters dialog—one for Axis Limits and one for Operation Limits?A. Axis Feed Rate limits are totally independent from the feed rate that you enter in the toolpath parameters. Typically, feed moves in your toolpath are interpolated in more than one axis. For example, if the tool is at 0,0 and you program a move to 1,1 at 1 in/min, the X and Y axes are each only moving at .707 in/min. The Axis Feed Rate limits refer to only the component of the motion that occurs in the selected axis. The Operation Feed Rate Limits, however, do refer to the feed rate that is entered in the Feed rate field when you create a toolpath.
Q. Will the Machine Definition Manager limit the tool planes available based on the angle increment of a rotary or a nutating rotary? For example, a customer has a machine with nutating rotaries and each rotary has an indexing resolution of 2 degrees. When you currently program Mastercam for these machines, the post must check to see if the plane that the user created is actually supported by the machining scenario.A. For the initial release of X, this has not been implemented. This is possible in future releases if the users want it.
Q. Why do we need axis combinations in the machine definition?A. There are frequently machines with more than one definition for the same axis. The most common examples are multi-turret, multi-spindle lathes, where each turret/spindle combination represents the same set of X-Y-Z axes, but which are coming from different parts of the machine. In other words, the orientation and location of the X axis changes when you move from the upper left turret to lower right turret. Axis combinations leverage the machine component tree that you build when you create your machine definition to let you pick and choose combinations of components. Each set of components has a complete set of axes, which you can name. When you're creating a toolpath, instead of having to choose spindles and turrets, you just select an axis combination. As your machining job progresses and you're machining with multiple turrets, it allows you to not worry about your coordinate system or axis orientations from operation to operation. This applies mostly to lathes and routers, but also to mills where a quill Z is used in addition to the initial Z axis. Every machine definition will have at least one axis combination, called Default, which is created when you save the machine definition. This combination is created automatically. In addition, you can create as many named axis combinations as you like. Individual components can be part of more than one axis combination, depending on your needs and machine complexity. The home position and reference points for a machine definition are actually saved as part of an axis combination, so to set the home position or default reference points for a machine, you need to click the Axis combinations button on the toolbar.
Q. When I’m creating a Lathe machine definition I see a new option to automatically update the WCS. What is that for?A. When you are creating a Lathe machine definition, the following option is available as part of the General Machine Parameters (in the Op limits/feed rates/axis orientation tab):
This option tells Mastercam to automatically align the WCS with the selected view whenever this particular machine is chosen. Most common lathe turning applications require that the WCS be set to Top. If you frequently need to manually change the WCS to Top, this option might be convenient for you. The Lathe Z = World Z option is useful if your lathe parts are typically drawn in a world coordinate system where the Z-axis is vertical, like a typical mill part. Select this option to have Mastercam automatically set the WCS so that you can create regular turning operations without transforming the geometry.
Q. Can you explain the Lathe Z = World Z option?“Lathe Z = World Z” is the name of a special view that is available in the View Manager when Mastercam Lathe is running. It lets you define a lathe part revolved about the world Z axis, but program it as it sits on a lathe. It flips Z to world X, X to world Y and Y to world Z. When you align the WCS to it, Mastercam maps the axes to a standard lathe coordinate system, so that you can use Mastercam’s standard lathe toolpaths to create 2D turning operations without transforming the geometry. The following picture shows the effect:
In your lathe machine definition, you can tell Mastercam to automatically switch to this view whenever that machine is selected, or you can access it in the View Manager as needed, just like any other view.
Q. Is this view always available in the View Manager?A. This view will only be displayed when a Lathe or Mill/Turn machine definition has been selected.
Q. How do I use other views that are relative to the new Lathe Z = World Z?A. Highlight the Lathe Z =World Z view in the View Manager and click the Relative button. You are prompted to pick which relative views you would like to use from a list.
|
