You need to measure X and Z Offsets for every tool in the job, using the F2/Measure key on the tool offset library screen. Setting the tool offsets will simultaneously locate the X axis stock zero point (i.e. the spindle centerline).
You will usually use the Part Setup screen to locate the Z axis part zero point (i.e. the end of the stock).
On the graph screen a rapid (red) move inside the part outline usually indicates a crash. However, rapid moves may be displayed below the part surface immediately before a tool change or at the end of the program. This is a normal consequence of canceling tool length compensation, and in this case does not necessarily indicate a crash.
The X axis controls the cross slide, for diameter dimensions. Positive X travel moves the tool tip away from spindle centerline, cutting larger diameters. Negative X travel moves the tool tip towards spindle centerline, cutting smaller diameters.
Depending on your machine, tools may approach the workpiece either from the front of the part (as on a manual lathe, and on most CNC lathes with a manual toolpost) or from behind the part (as on most turret lathes).
On gang tool and dual-turret machines it is common to have tools which approach from both sides of the part. In that case, however, you (or the machine builder) will have to decide which is the "front side" and which is the "back side". Tools on the front side will cut in positive X coordinates; tools on the back side will cut in negative X coordinates.
The Centroid control can be set up so that its jog pendant and Setup screen illustrations are consistent with either type of machine. With the tools in front, for example, the X- jog button is on top and the X+ jog button is on the bottom. With the tools in back the jog keys are reversed.
However, when viewing part geometry and programming parts, you always look at the "top" or "back" half of the part, as if the tools cut from behind the workpiece. Thus the cut shown at right would always be programmed as a Counterclockwise Arc, with Cutter Compensation to the Right of the workpiece, even if the tool was actually in front and the carriage was going to arc clockwise to make the cut.
Stated another way: on the machine, on the jog pendant, and on the Setup screens, X+ might be down or towards you if the tools are in front. In part programming, X+ is always up.
Cutter Compensation is the process of moving the cutter closer to the part on diagonal and arc moves, to account for the fact that the insert has a radiused tip. Cutter compensation is not necessary on straight diameters and straight faces.
Compensation can be done in advance, by writing G codes that place the cutter closer to the part on diagonal and arc moves. This is called precompensating.
Alternately, compensation can be done at run time by including the G41 and/or G42 codes in the G code program. This is G code cutter compensation.
If a program is precompensated, and you find that the actual tool nose radius is not what you expected, then you must rewrite the G codes to precompensate them with the correct radius, then run the new G codes.
If a program uses G code cutter compensation, and you find that the actual tool nose radius is not what you expected, then you need only change the radius listed in the Tool Offset Library, then rerun the same G code program you ran before.
Use compensation Right (G42) for outside diameter cuts while moving towards the chuck; for back face cuts while moving towards centerline; and for front face cuts moving away from centerline.
Use compensation Left (G41) for inside diameter cuts while moving towards the chuck, and for front face cuts while moving towards centerline.
An Intercon part program consists of two files on the computer. One has the extension .LTH, and contains all of your responses to the prompts (everything you see on the screen while you are in Intercon). The other file has the extension .CNC, and contains the resulting G codes.
Intercon automatically saves both files whenever you choose Post.
When you edit the part program in Intercon, you are editing the .LTH file.
When you run the job, you are running the .CNC file.
When you press F6/Edit from the main screen, you see the CNC file (the G codes) in the text editor. Any changes you make on this screen will be lost next time you go back to Intercon and post the part. This is because Intercon rewrites the CNC file based on the information in the .LTH program file. Intercon never tries to read back the CNC file to look for changes you may have made there.
There are three general approaches to programming a part with Intercon:
For simple parts (one or two features, straight or only shallowly tapered, with no significant chamfers or radiused corners between them) the Turning cycle will be most expedient.
Turning Cycle Example
The Turning canned cycle does both turning (OD and ID) and facing (front and back faces). It will automatically make any necessary rapid move to the starting point of the cycle. Cuts can be tapered, but steep tapers are not recommended due to the amount of time spent off the part. The Turning cycle has no provision for radiused corners.
In the sample illustration above, there would be two Turning cycles: one to face the end of the part, and one to turn down the outside diameter. If the corner between the two needed to have a radius, it could be done later with separate line and arc moves, as in the example below.
For more complex parts (steep tapers, chamfers, and radii) which can be cut in a single pass (e.g. rework on a part which is already shaped, or where only a small amount of material needs to be removed) then building the whole path with Line and Arc moves will be simplest.
Line and Arc moves are not self-contained the way canned cycles are. There is no automatic positioning move to the beginning of the cut. Instead, you must insert Line moves (Rapid or Feedrate as appropriate) to get the cutter to the beginning of the cut; then insert Line and Arc moves to make the cut; then insert one or more Rapid moves to move the cutter clear of the part.
In the sample illustration above, to make a radius on the corner, there would probably be four moves: A Rapid move just short of the material near the start of the radius; a Line move to touch the material at the start of the radius; an Arc move to cut the radius itself; and a Rapid move to get the cutter clear. Tool nose radius compensation could be included. If it is not, then the programmed radius should be increased by the radius of the cutter tip.
For complex parts which require multiple cutter passes to remove all the material, the Profile cycle will be most effective.
The Profile cycle is a powerful tool for roughing and finishing nearly any shape of part. However, it has a few requirements you have to observe.
By programming straight to the finished profile, it may seem as
if you are programming the cutter to plow out all the material
in one impossibly deep cut. Indeed, if these Lines and Arcs
were not contained inside a Profile cycle, that is exactly what
would happen. But the Profile cycle will automatically make
all the roughing passes needed to work down from the starting
(uncut stock) diameter to the finished profile.
In the sample illustration above, the program would start with a Turning cycle to face off the end of the stock, then would use a Profile cycle to turn the OD profile starting with the radius on the rightmost corner. The Start point would be just off the upper right corner of the uncut stock. The Profile definition would include a Line moving straight in the X- direction to a diameter at or below the beginning of the first radius; then a Line moving straight in the Z- direction to the end of the stock (the beginning of the radius); then a CCW Arc around the radius; then a Line in the Z- direction to the beginning of the large radius; then a CCW Arc around the large radius; then another Line Z-; then finally a line in the X+ direction to the stock diameter. The small CW radii before and after the large arc could be inserted automatically using the Connect Radius feature on the moves which lead into them.
Some other fields on the Profile cycle screen require a little explanation:
"Stock to Leave" on X and Z are the finish allowance. The cycle will automatically shift the given finish profile in X and Z to obtain the boundaries of the roughing passes. In general, you should enter a finish allowance only on X when doing a diameter turning Profile, and only on Z when doing a facing Profile. To understand why, imagine you are using a button cutter to turn a diameter profile that includes a steep-walled groove. If you enter +.010" for "Stock to Leave" on the Z axis, then the control will move the left wall of the groove to the right 0.010" for rough cuts (okay so far), and it will also move the right wall of the groove to the right 0.010". The rough cuts will now overcut the right side of the groove.
In the example pictured above it would be okay to include a positive finish allowance ("Stock to Leave") on both X and Z, because there are no obstructions to the right or outside of the profile.
"Rapid Between Cuts" says whether each plunge to the next depth may be made as a Rapid move, or whether plunges should be made at cutting feedrate. If the Profile starts clear of the end of the part, and doesn't have any pockets (cavities, shadowed areas, ...) then it is always safe to choose Rapid Between Cuts = Yes, because the plunge moves will never touch the part. If, on the other hand, the Profile starts in the middle of the part, or includes pockets, then you should choose Rapid Between Cuts = No.
Every series of freestanding Line and Arc operations should be preceded by a Rapid operation, to bring the cutter to the starting point of the first line or arc.
You generally do not need to include a Rapid operation before a canned cycle (e.g. turning, threading, profile, etc.). Intercon will automatically put in a rapid move to the starting point of the cycle.
However, if you are doing consecutive canned cycles on opposite sides of an obstacle (e.g. a raised rib on the part diameter), you may have to add a Rapid move to get over the obstacle.
On gang tool machines, where the carriage moves directly from tool to tool without returning to a tool change position, you almost always have to insert one or two Rapid moves when you change tools: one move to get the previous tool clear of the part, and usually a second move to bring the new tool into position. Always visualize what would happen if the carriage moved directly from the end of one operation to the beginning of the next. If something is in the way, then add a Rapid move (usually straight Z+) to get clear.
The most reliable way to change tools on a gang tool machine is as follows:
To transfer an Intercon program from one control to another, or to or from an offline programming computer, you need to put the .LTH file on a USB drive.
To save the program file to a USB drive:
To load an Intercon program from a USB drive:
Ordinarily you start jobs by pressing CYCLE START from the main screen, or any other screen where the message box prompts "Press CYCLE START to start job".
When running a new job or new setup for the first time, keep your hand on the feedrate override knob during the initial approach move after each tool change. As the tool rapids towards the part, slow it down by turning down the feedrate override. When the tool is about one inch from the part, pause it by pressing FEED HOLD. Check the DRO position display for the each axis. If the position shown there appears to match the position of the tool in front of the part, all is probably well: press CYCLE START to continue. If the position shown on the DRO does not match the position of the tool (especially if it reads higher), something is wrong: press CYCLE CANCEL and review your tool measurements and part zero setting.
You can cancel a job at any time by pressing EMERGENCY STOP, CYCLE CANCEL, or TOOL CHECK.
EMERGENCY STOP will stop motion immediately, release servo motor power, and shut off the spindle and coolant. Once the crisis is past, you can release E-stop and use the jog keys or TOOL CHECK key to move the tool clear. The control's main screen will be displayed (with Setup, Load, MDI, etc. options). The G codes which were running when the job was canceled will remain on the screen until you choose some other screen.
CYCLE CANCEL will stop motion immediately and shut off the spindle and coolant. Servo power will remain on. You can use the jog keys or TOOL CHECK key to move the tool clear. The control's main screen will be displayed (with Setup, Load, MDI, etc. options). The G codes which were running when the job was canceled will remain on the screen until you choose some other screen.
TOOL CHECK will decelerate to a smooth stop, then shut off the spindle and coolant. The control's Run/Resume screen will be displayed, ready to pick up where you left off. If you choose, you can press ESC twice to return to the main screen.
In any of these cases, you can resume the uncompleted job on the move where it was interrupted by using the Run/Resume option. From the main screen, press F4/Run, then F1/Resume. If you wish, use the jog keys to move the tool close to where it was when you stopped the job. Press CYCLE START to resume at the beginning of that line of G codes. The control will automatically restart the spindle and coolant as needed, move X and Z to the beginning of the move, and resume running.
If you want to restart the job at some other point than where you interrupted it (for example, if the tool broke several moves back) use the Run/Search option. From the main screen press F4/Run, then F2/Search. You can enter a line number (the default will be the line where the job was interrupted), a block number (N number), or a tool number. The control will locate the place you choose and start running the job from there.
If you are uncertain whether the search point you ask for is really what you want, you can get a graphic preview from the Search screen: type the line number, block number, or tool number, but do not press Enter yet. Press F8/Graph instead. The part will display with blue dotted lines for everything which is being skipped over, and with the usual yellow and red lines beginning at the search point. Press ESC to leave the Graph screen, then either press Enter (or F10 or CYCLE START) to accept the search, or enter a different search point if needed.
Except on gang tool machines, Intercon usually inserts a G28 code at the beginning and end of every CNC program, and also at every tool change. This brings the carriage out to a preset return position where you can change tools manually, or where the tool turret can rotate without interference.
By default, this tool change position is at the machine zero position: cross slide all the way out and carriage all the way to the right, where the machine finds home when first powered on.
On a large machine, you may not want to take the time for the carriage to go all the way down to the end of the bed. If you are working with a tailstock advanced, it may not even be possible to go there.
You can change the G28 tool change position at any time, from the Part Setup screen. It is usually best to let X come all the way out to machine zero, but change Z to suit the job:
Back to on-line tutorials page
Copyright © 2012 Marc Leonard
You are welcome to print out this tutorial for your own use and for non-commercial distribution, as long as you include this copyright message.
Last updated 09-Nov-2012 MBL