Centroid software version 2.70

Using the features of control software version 2.70

Accelerated Graphics

New in v2.66

To enable the accelerated graphic preview, set Machine Parameter 260 to a value of 1.0:

  1. Press F1 for the Setup screen
  2. Press F3 for the Configuration screen
  3. Enter the configuration password
  4. Press F3 for the Parameters table
  5. Press F8 twice to see Parameters 200-299
  6. Select Parameter 260 and enter 1.0.
  7. Press F10 to save
  8. Press ESC as needed to return to the main screen

When you press F8/Graph, you will see the accelerated graphics interface. A "hints" box will appear on top of your image; you can press F9 ("Zoom All") to redraw and blank out the hints box.

With the accelerated interface you can:

Command recall at the MDI prompt

New in v2.36

To recall previous MDI commands, simply press the up and down arrow keys at the MDI prompt.

Inverse time feedrates for Mill controls

New in v2.36

Inverse time feedrates are generally used in 3D CNC programs consisting of many short G1 vectors. They are particularly useful in 4-axis and 5-axis programs where the feedrate in units/minute can be difficult to calculate.

Inverse time feedrates specify the feed as vectors (i.e. G1 moves) per minute.

If all vectors are the same length (or at least the same tooltip-over-part distance) then a single feedrate value can be used throughout.

More commonly the vectors are differing lengths, and every line must contain its own feedrate. The benefit over inch/minute feedrates is that the feedrate can be calculated based on tool-over-part distance without regard for fourth and fifth axis rotary movement.

Distance-to-go DRO

New in v8.20

The distance-to-go DRO is not displayed by default.

To turn on the distance-to-go DRO:

  1. Press F1 for the Setup screen
  2. Press F3 for the Configuration screen
  3. Enter the configuration password
  4. Press F3 for the Parameters table
  5. Press F8 to see Parameters 100-199
  6. Select Parameter 143 and add 8.0 to its previous value.
  7. Press F10 to save
  8. Press ESC as needed to return to the main screen

Improved Text Editor

The F6/Edit key uses a new text editor, called NEdit. Click here for information on using NEdit.

Runtime Graphics

New in v8.10

The runtime graphics feature is turned off by default.

To turn on runtime graphics:

  1. Press F4 for the Run menu
  2. Press F10 to turn on runtime graphics
  3. Press CYCLE START to start the job

Once turned on, the runtime graphics feature stays on until turned off, or until the control power is switched off.

You can change the default so that runtime graphics are on every day (at power-up) unless you explicitly turn them off.

To make runtime graphics be on by default:

  1. Press F1 for the Setup screen
  2. Press F3 for the Configuration screen
  3. Enter the configuration password
  4. Press F3 for the Parameters table
  5. Press F8 to see Parameters 100-199
  6. Select Parameter 150 and change it to 1.0
  7. Press F10 to save
  8. Press ESC as needed to return to the main screen

If runtime graphics are on by default, you can still turn them off using the Run menu as described previously.

When runtime graphics are on, you can press F8 as the job runs to switch back and forth between the graphics display and the G code display.

G76 Fine Boring Cycle for Mill controls

New in v2.32

The fine boring cycle works just like the G85 boring cycle, except that when the tool reaches the final depth, the control stops and orients the spindle; moves a specified distance in the Y+ direction; and retracts from the hole with the spindle stopped.

This feature requires that your machine be able to orient the spindle in response to an M19 command. Generally, mills with automatic tool changers can do this, and all other machines cannot. If you are not sure whether your machine has a spindle orient, just try the M19 command as described below.

As of version 2.36, the direction of retract is fixed (Y+), so you must set up the boring bar so the cutter tip faces you (points in the Y- direction) when the tool is inserted with the spindle in the orient position.

To orient the spindle in preparation for inserting or setting up the boring tool:

  1. Press F3 for the MDI prompt
  2. Enter the command "M19"
  3. Press CYCLE START

Rotated coordinates (fixture compensation) for Mill controls

New in v8.00

Coordinate rotation applies to the X and Y axes only, to compensate for a fixture that is out of square. It does not apply to the Z axis, and so cannot compensate for a fixture that is not level.

Each coordinate system (fixture) has a separate rotation angle. If you are working with multiple vises, you will want to measure the rotation angle separately for each one.

You can measure coordinate rotation either before or after you set the part zero location on the X and Y axes. If you set the part zero location first, then measure coordinate rotation, the rotation is done around part zero (X0 Y0). That point will remain fixed, while all other points rotate around it.

If you measure coordinate rotation first, then set the part zero location, the control will compensate for rotation as it locates part zero. Thus, if you will be touching off on a position that is not X0 Y0, you should measure coordinate rotation first.

Coordinate system rotation can be measured with a touch probe or manually.

To set coordinate system rotation with a touch probe:

  1. Press F1 for the Setup screen
  2. Press F1 for Part Setup
  3. Press F8 for the Coordinate System Rotation screen
  4. Press F6 and/or F7 as needed to select the correct coordinate system
  5. Press F1 as needed to select the orientation of the surface you are going to probe
  6. Jog the probe in front of the surface near one end
  7. Enter the distance (plus or minus) which the probe should move parallel to the surface between measured points. For example, if you are going left to right across the front of a 6" vise jaw, starting about 1/4" in from the left end, then you would enter 5.5" for the distance.
  8. Enter the clearance amount needed in Z to jump over any obstacles between the two points. This is an incremental distance above whatever Z level you start out at. If there are no obstacles, you can enter 0.0 for the clearance amount.
  9. Select "Movement Between Points" to be Auto if you want the control to do all probe movement automatically. Select Manual if you want to jog the probe from one point to the other yourself.
  10. Press CYCLE START to start the probing cycle. The control will automatically measure one point directly in front of the probe, then move over by the distance you entered and measure another point. It will then compute the coordinate rotation angle and enter it for the current coordinate system.
  11. Press ESC to return to the Part Setup screen

To set coordinate system rotation manually:

  1. Compute the rotation angle: angle = arctan(Y distance / X distance). For example, if you sweep a 6" wide vise jaw with an indicator, and find that the jaw moves towards you 0.0015" as you sweep from left to right, then the angle is arctan(-0.0015/6), or -0.014°.
  2. Press F1 for the Setup screen
  3. Press F1 for Part Setup
  4. Press F9 for the Workpiece Coordinates screen
  5. Press F2 to edit the table of workpiece coordinate origins
  6. Enter the computed rotation angle under the appropriate coordinate system(s)
  7. Press F10 to save
  8. Press ESC as needed to return to Part Setup or the main screen

If a coordinate rotation is set for the current coordinate system, a rotation icon will appear between X and Y on the DRO display.

To clear out the rotation corrections for all coordinate systems:

  1. Press F1 for the Setup screen
  2. Press F1 for Part Setup
  3. Press F8 for the Coordinate System Rotation screen
  4. Press F4 to clear all rotations
  5. Press ESC as needed to return to Part Setup or the main screen

Outside contour (cam) digitizing

New in v7.50

CAM digitizing traces a single constant-Z contour around the outside of a raised model. It then produces G codes which will cut the contour, optionally taking multiple cutter passes.

Programmable AUX keys

New in v8.20

You can use the AUX1, AUX2, etc. keys to quickly set part zeros, power axes on and off, call up one-shot conversational canned cycles, and perform other tasks.

Machine Parameters 188 and following select AUX key functions. Parameter 188 is for AUX1; Parameter 189 for AUX2; Parameter 190 for AUX3; and so on. Set the parameter value to select the function you want to assign to the corresponding AUX key.

Possible values are as follows:
No Function0Set XYZ Zero16
Enter X Axis Position1One Shot Bolt Hole Circle17
Enter Y Axis Position2One Shot Drill Array18
Enter Z Axis Position3Jog X+21
Set Position, Absolute4Jog Y+22
Set Position, Incremental5Jog Z+23
One Shot Drill6Jog 4th +24
One Shot Circular Pocket7Jog 5th +25
One Shot Rectangular Pocket 8Jog X-31
One Shot Frame 9Jog Y-32
One Shot Face10Jog Z-33
Free Axes14Jog 4th -34
Power Axes15Jog 5th -35

The "Enter Axis Position" functions must be used with one of the "Set Position" functions. For example, with Parameter 188 set to 1.0 and Parameter 191 set to 4.0, you could press the AUX1 key to enter an X axis position, then press AUX4 to accept and set the position.

Quick Teach and new field editing features in Intercon

New in v8.00

While editing any Intercon operation, you can plug in the current DRO position from the X, Y, or Z axis simply by typing that letter.

For example, to enter a Rapid move to the current tool position:

  1. On the Insert Operation screen, press F1 for Rapid
  2. With the End X coordinate highlighted, press the X key
  3. With the End Y coordiante highlighted, press the Y key
  4. With the End Z coordinate highlighted, press the Z key
  5. Press F10 to accept the operation

You can display a live DRO in the lower left corner of the screen for reference purposes. Press F9/Teach to display the live DRO; Press F9/Teach again to hide it. You do not have to have the live DRO on the screen in order to use the quick Teach feature.

There is no longer any way to zero the DRO (temporarily change part zero) within Intercon for the Teach feature. Instead, you must set the part zero where you want it, using the regular Part Setup screen, before entering Intercon.

The method of editing field values in Intercon has changed slightly. If you want to enter a new value, replacing any previous value, you just start typing as before. However, if you want to modify the previous value without replacing it (e.g. to change one digit or to add or remove a minus sign) you now press the Enter key, then move the cursor where you want it using the arrow keys. Previously you just used the right arrow key immediately without pressing Enter first.

Cleanout cycle for irregular pockets in Mill Intercon

New in v8.00
Spiral path and islands new in v1.26

Cleanout is a new canned cycle in Intercon. The Cleanout operation itself contains all the usual pocketing information: depth, number of passes, rough and finish cut amounts, etc.. It does not contain any information about the horizontal (XY) dimensions of the pocket.

The Cleanout operation is followed by a bracketed series of Line and Arc moves which define the outline of the pocket. The first Line simply establishes a starting point. The subsequent Line and Arc moves become the finished outline. If the outline is not closed (the last move does not return to the starting point) Intercon will automatically close it with an assumed straight line.

Drill Arrays (rectangular pattern)

New in v8.00

Mill Intercon's Drill, Bore, and Tap cycles now allow rectangular arrays.

You enter the position of the first hole, then the number of holes and hole spacing along the X and Y axes.

A "skip list" allows you to leave selected holes out of the pattern.

Drill Repeats for multiple operations on the same set of holes

New in v8.00

If you have a pattern of single holes (entered with separate XY locations, rather than as Arrays or Bolt Hole Circles), you can now do additional operations on the same set of holes without having to reenter the coordinates.

For example, you would enter individual Drill operations to center drill each of a dozen locations. You could then change tools and use a Drill Repeat to drill through at each location. You could then change tools again and use Tap Repeat to tap all those locations. If you later needed to correct the coordinates of one or more holes, you would only need to change the original center-drilling holes. The through-drill and tap holes would move automatically.

Extended in-line calculator in Intercon

New in v8.00

Intercon has supported in-line arithmetic since version 6.00. However, its utility has been limited by the 10-character input box that your formula had to fit in.

In the new software, simply press '=' while entering any number. The extended expression box appears, with room for almost any calculation you may want to make. Enter the expression, then press Enter or '=' again. The calculated result is plugged into your operation and you are ready to proceed.

Improved Intercon Math Help

New in v8.00

Variables and arithmetic in G codes

New in v8.00
IF/THEN/GOTO new in v8.10

CNC Macro Programming Examples

Improved MPG handwheel jogging

New in v8.00

MPG jogging at higher speeds will automatically move more smoothly with the new software.

To take advantage of this, you may wish to enable MPG jogging on the 0.010" (x100) increment. To do so, set Parameter 19:

  1. Press F1 for Setup
  2. Press F3 for Configuration
  3. Enter the configuration password
  4. Press F3 for Parameters
  5. Select Parameter 19 and change it to 2.0
  6. Press F10 to save
  7. Press ESC as needed to return to the main screen

Note: at higher speeds, the control will not respect exact increments as you turn the handwheel. Instead it will switch to a continuous-motion mode where the wheel controls speed. Once you slow back down to a low speed (discrete clicks) then the control will once again move by the exact increments requested.

Axis load meters on DRO display

New in v8.00

To turn on axis load meters, set Parameter 143:

  1. Press F1 for Setup
  2. Press F3 for Configuration
  3. Enter the configuration password
  4. Press F3 for Parameters
  5. Press F8 to see Parameters 100-199
  6. Select Parameter 143 and change it to either 1.0 (for load meters without outlines) or 3.0 (for load meters with outlines)
  7. Press F10 to save
  8. Press ESC as needed to return to the main screen

Search by tool number (T)

New in v7.08

The Run/Search screen now allows you to start the job at a specific tool number, without having to know the line or block number.

  1. Press F4 for the Run screen
  2. Press F2 for Search
  3. Enter a tool number using the letter T
  4. Press CYCLE START to begin at that tool change

The job will begin at the first tool change where that tool is loaded. If the same tool is called more than once, and you want to start at a later tool change, you must enter the line or block (N) number to search to the later tool change.

Graph only a selected range of your job

New in v7.00

On the graphic preview screen, press F3 to set the graphing range.

This can make it easier to view specific features of a complex part which has many overlapping cuts.

You can enter either line numbers or block (N) numbers at which the graphing should start and end. If you leave the Start point blank, graphing will start at the beginning of the program. If you leave the End point blank, graphing will run to the end of the program.

If you have entered start and end points to limit the graphing range, then want to return to viewing the entire part, press F3 again and delete (blank out) the start and end points.

Smart Search

New in v6.00

You can search to any point in the job and begin running there, with the correct feedrate, Z depth, spindle and coolant, tool length and cutter compensation.

Press F4 for the Run menu, then F2 for Search. Enter the line, block (N), or tool (T) number where you want to start, then press CYCLE START.

If you canceled the previous job before it finished (e.g. with CYCLE CANCEL, Emergency Stop, or TOOL CHECK) then the control will display the line number which was running when you canceled the job. You can accept this number to restart where you left off, or you can enter any other search point you choose.

Fully functional TOOL CHECK

New in v6.03

While a job is in progress, press TOOL CHECK to interrupt it.

The axes will decelerate to a smooth stop; the Mill's Z axis will pull up to the tool change position; and the spindle and coolant will switch off. The control will automatically display the Job Resume screen (F4/Run, F1/Resume).

On a Lathe there is no automatic retract when you first press TOOL CHECK during a job. However, once the job is paused, if you press TOOL CHECK a second time, the carriage will retract to the tool change position.

You can clear chips and measure the part. You can even replace a worn or broken tool, and can go to the Offset Library to measure or enter new tool offsets.

To resume running where you left off, press CYCLE START from the Job Resume screen. You may wish to jog close to the part first, to save time that would otherwise be spent moving to the part at your cutting feedrate.

When you press CYCLE START to resume on a Mill control, the control will restart the spindle and coolant; move X and Y over the beginning of the interrupted cut; move Z down to cut depth; and resume running the program normally.

When you press CYCLE START to resume on a Lathe control, the control will restart the spindle and coolant; move X and Z directly to the beginning of the interrupted cut; and resume running the program normally.

If you need to back up and restart at an earlier point in the program (for example if the tool broke several moves back) you should press ESC to leave the Resume screen and instead press F2 for the Search screen. The Search line number will default to the line which was running when you pressed TOOL CHECK. You can edit this number to be a few lines back. If you are unsure of the correct starting line, you can preview the search with F8/Graph. When ready, press CYCLE START to start on the chosen line.

Extended workpiece coordinate systems

New in v7.08

There are now 18 independent part locations, plus 4 reference return points.

Selectable plunge ramp angle in Mill Intercon's canned cycles

New in v7.08

Intercon's Rectangular Pocket, Circular Pocket, and Frame cycles now allow either a ramped plunge at any angle you choose, or a straight-down plunge.

The default is a ramped plunge. The Plunge Angle defaults to 0.0, which means to use a default of 45°. If you choose, you can change the Plunge Angle to suit your cutter: 10° would be a very shallow ramp; 80° would be a very steep one.

If the pocket is not wide enough to allow the cutter to ramp down to your chosen cut depth at your chosen angle, Intercon will zig-zag down in multiple ramps.

If your tool is not suitable for downward cutting at all, choose a straight plunge and insert a drilling operation before the pocket or frame, to drill out the plunge point. For pockets, the plunge will always be in the center of the pocket. For frames, the plunge will be near the back left corner (if climb milling) or the back right corner (if conventional milling). It will be a cutter radius away from the back wall, and will be inside any corner radius. If in doubt about where the plunge point is for a Frame mill, check its endpoint as displayed in the program listing on the left side of the screen.

Thread Milling canned cycle in Mill Intercon

New in v6.02

Intercon includes a canned cycle for Thread milling.

Entering your program in Intercon, press F5 for Canned Cycles, then F8 for Thread. Fill in the relevant thread dimensions.

The Diameter dimension refers to the final cut taken by the thread mill. For internal threads, this should be the major diameter. For external threads, this should be the minor diameter.

You can request multiple cutting passes, but any after the first are spring passes (retracing the same toolpath as the first pass). If you need to remove more material than your thread mill can cut in one pass, you should enter two or more Thread cycles: the earlier ones cutting to smaller diameters (for internal threads) or larger diameters (for external threads).

The Thread cycle cuts the threads in or on an existing hole or boss. You may need to include Drill, Circular Pocket, and/or Frame cycles before the Thread cycle.

If you choose a single-point cutter, the Thread cycle will spiral down in as many turns as are required to reach the depth you enter.

If you choose a full-form cutter, the Thread cycle will do only one spiral pass, regardless of depth. It assumes the cutter insert has enough teeth to cut the entire thread.

Peck tapping added to the rigid tapping option

New in v7.06

If you have the rigid tapping option on your machine, Intercon will now allow you to do peck tapping.

On the Tapping canned cycle screen in Intercon, simply enter a depth increment less than the total depth of the hole. Intercon will output multiple G84 tapping cycles, causing the tool to tap down by the requested depth increment; reverse back to the surface; run forward down another increment; and so on to the full depth. Each successive peck will synchronize to the previously cut threads.


Copyright © 2011 Marc Leonard
You are welcome to print out this page for your own use and for non-commercial distribution, as long as you include this copyright message.
Last updated 21-Apr-2011 MBL