Setting up a Machine Configuration

How to's for using NCPlot

Setting up a Machine Configuration

Postby scottmartinez » Sat Sep 02, 2006 10:57 am

Setting up a Machine Configuration

In order for the graphics viewport to properly display your G-Code program, it must first know a few things about the machine you intend to run it on. Since there are many different types of machines and CNC controls, NCPlot has options that allow it to mimic the way your particular CNC control reads G-Code. NCPlot doesn't recognize every G or M Code that your control does, but it should still be able to give you a good representation of your programs toolpath.

NCPlot comes with a handful of predefined machine configurations. These configurations represent the most common settings for a CNC control and should be good enough to get you started. Even so, you should check that these settings match the way your control works.

To open the machine configuration dialog, click the menu "Setup", then click "Machine Configuration". This dialog is made up of several tabs, the first tab you see is labeled "Machine Type". This tab has settings that define the basic setup of your machine.


Machine Type Tab

You must first select between Mill and Lathe. Choosing one or the other will change or enable/disable other settings on the dialog. If you selected Mill, you now have the option to select between Vertical spindle and Horizontal spindle. If you selected Lathe, you now have the option to select between Radius Coordinate values and Diameter coordinate values. This setting determines how NCPlot interprets the X/U axis command values. The Lathe type also has a check box that allows the direction of G2/G3 arc commands to be reversed.

Also on this tab is a setting called "Default Program Folder". This setting can be set to point to a folder where the G-Code programs for this particular machine configuration are stored. Say for example you have a configuration for a Makino vertical machining center. All the programs for it are stored at "C:\Jobs\MakinoVMC". Simply set the default program folder to this folder, then any time you want to open a file, the "File Open" dialog will open right to this folder. Since this setting is part of the machine configuration, you can specify a different folder for each configuration.


Control Options 1 Tab


This tab contains some of the most important settings for determining how your G-Code programs are interpreted. First off is the "Rapid Type" setting. This setting should be set to match how your machine responds to a multiple axis simultaneous rapid move. If your machine handles this as "Interpolated", then all three axes will always arrive at their endpoints at the same time. If the axes reach the endoints one at a time, this would be "Non-Interpolated" sometimes called "Dog-Leg". Some controls use a third method which is generally safer than the other two. This method will always move the Z axis by itself, either before or after the X & Y axes depending on which direction the Z is going.

The "Coordinate Resolution" setting determines how many decimal places to assume when a command value is given without a decimal point. For example, if you have a program that has commands like "Z-152500", then you would want to set the coordinate resolution to "0.0001" so that this would be properly interpreted as "Z-15.2500". Here's some more examples:

Command value Coordinate Resolution Interpreted value
X25 0.001 X0.025
X1 1.0 X1.0
Y1250 0.0001 Y0.1250
Y1.250 n/a Y1.25 Since a decimal point was specified, the resolution setting is disregarded.

The arc settings determine how G02 and G03 arc commands are interpreted. If your control uses absolute arc centers, then check the box that says "Absolute Arc Centers". When checked, I, J and K values in a G02 or G03 command represent the location of the center of the arc in the current work coordinates. When unchecked, the I, J and K values represent the distance from the start point of the arc to the center point of the arc.

If your control uses absolute arc centers, it may also treat the center locations as modal. If this is the case, the control remembers the last center point you programmed and you don't have to include an I, J or K value in every arc command. If you have a control that behaves this way, check the box that says "I/J/K values are modal".

When you command an arc using IJK arc center designation, it's not uncommon for there to be a small difference between the arc's start radius and end radius. That is, the difference between the distance from the start point to the center and the distance from the end point to the center. Most controls will handle this without a problem up until the difference reaches a certain amount. Whether this amount is fixed in the control, or is parameter settable, you can enter this amount into the "Arc Tolerance" setting. When NCPlot encounters an arc where the start and end radius is different by more than this amount, an error will be displayed.

When NCPlot begins to backplot a program, it starts from a fixed G-Code state. That is, certain G-Codes are active by default such as G00, G90, G54 etc. While this is acceptable for most controls, you may have a machine that defaults to some other active state, like G91. The "Initial State" setting is used to define the default state of your control. For example, if your control defaults to G91 you simple add "G91" to the Initial state setting.

The "Top Viewport" rotation setting allows you to re-orient the graphics display to match the way the part appears from the operator side of the machine. This is simply a convenience setting that only affects the graphics view.


Control Options 2 Tab

If you intend to backplot programs in the Custom Macro B format you should set the ATAN function format. This setting determines the format that is expected when an ATAN function is encountered in the program. In general, Fanuc controls expect the two operand format, while Mitsubishi controls expect the single operand format. For others, check your control documentation to determine the correct setting.

The "G-Code Macros" setting is a list of G-Codes that NCPlot will call as subprograms when they are encountered in a program. When encountered, all other address values are written to local variables and a specially named subprogram is loaded. The name of the subprogram that is loaded is in the format "Gxxx.PRG", where "xxx" is the G-Code value times 10. For example, if you have G12 in the G-Code macro list and NCPlot encounters the block "G12 X0 Y0 I0.5", a subprogram named "G120.PRG" must be in the configuration folder. The values for X, Y and I are saved to local variables and can be used by the subprogram to simulate the motion for a G12 command. This method allows you to simulate G-Codes that are not handled internally by NCPlot.


G/M Codes Tab

If you plan to backplot programs that use M98 for subprograms, then it's very important that you set the M98 command format to match your control. There are five different settings, so if you're not sure which one to use, you should consult your control's programming manual.

If your control supports M-Code activated mirror image, then use this tab to set the M-Codes that are used to activate this function.


Viewport Colors Tab

This tab contains settings that define the colors used to draw the backplot. You first must decide if you want to color by G-Code, or color by tool. To select one, check the box next to the header describing the method you want to use. When "Color by G-Code" is selected, the entities on the graphics viewport be will colored according to the type of motion it represents. There are 4 basic types of motion: G00 Rapid move, G01 Feed move, G02 Clockwise arc and G03 Counterclockwise
arc. Each of these types of motion may be assigned a different color.

The "Color by Tool" option draws the backplot with different colors representing the range of motion for each tool used in the program. The "Unspecified Tools" color is used when the program commands motion before the first tool change. The color list contains the colors to use for each tool. The first color in the list is used after the first tool change, the second color after the second tool change, etc. If there are not enough colors in the list for all of the tool changes in the program, the "Unspecified Tools" color will be used for any remaining tool changes. You may also specify the type of command that is considered a tool change, either the M06 command or a T-Code.

In addition to the entity colors, you can also specify the background color of the graphics viewport as well as the color of entities that are selected.


Work Offsets Tab

Just like your machine can accomodate multiple work offset coordinates, NCPlot can also be configured to recognize multiple work locations. This gives a backplot that accurately represents a multiple fixture setup.


Rotary 4th Axis Tab

If your machine has a rotary 4th axis, use this tab to define the settings for it. First, set the "4th Axis Identifier" to specify the letter address that commands the 4th axis. The most common settings are an "A" or "B" axis. Next, set the orientation of the rotary axis by specifying whether it rotates around the "X" or "Y" axis. By definition, an
"A" axis rotates around the "X" axis and a "B" axis rotates around the "Y" axis. You must also set the "Coordinate Resolution" setting for the 4th axis command values. This works the same way as the setting on the "Control Options 1" tab.

The "Rotary Centerline" settings can be used to specify where on your machine the rotary axis is located. This tells NCPlot where the center of rotation is located on the machine.
User avatar
scottmartinez
Site Admin
 
Posts: 215
Joined: Sat Mar 11, 2006 8:49 pm

Return to Tutorials

Who is online

Users browsing this forum: No registered users and 3 guests

cron