Looking for G-Codes for EZTrack - problem is that when facing a part for machining the machine will make it around four corners but when program steps in to make another pass - it bombs out at first arc in second pass.
Using I and J coordinates for interpolation? Should I be using R (radius) instead or is there a preperatory command that I should be using to complete multiple passes? List of all gcodes with explanations and syntax usage would be very helpfull (UG postprocessor too!)

Thanks
Ron

I do not remember a G & M code list ever published for the EZTRAK. But I know that the BOSS 8 or 9 post for EZCAM and FEATURE CAM worked very well. This is because the EZTRAK software was based on these earlier machines. If you ever write a program on the TRAK in conversational and load it to the BMDC, then press the minus key, you will see how the BMDC converted it to G & M code.

If you ever saw a program created by EZCAM for a BOSS 8, it is very simple. Most moves are G0, G1, G2, G3, and the drilling canned cycles. My EZCAM (MAC based for my BOSS 9) did not do cutter comp. You put in the tool diameter in the tool table and it created the path compensated by that radius. I had to add G41, G42, and G40 myself as well as the approach and departure moves.

You need someone to print a post document which shows all the details so you can copy it into your post.

George

This should do the trick.

TM



MOTION
*G0 Rapid Traverse
G1 XYZ Linear Interpolation (Feed)
G2 Circular Interpolation, CW
G3 Circular Interpolation, CCW
G4 Dwell
G12 Helical Interpolation, CW
G13 Helical Interpolation, CCW
G22 Circular Interpolation, Fillet Input CW
G23 Circular Interpolation, Fillet Input CCW
*G8 Deceleration Override OFF
G9 Deceleration Override ON
G99 Deceleration Override, Single Block
G74 Single Quadrant Circle Input ON
*G75 Multi-Quadrant Circle Input ON
PLANE SELECTION
*G17 XY, Plane Designation
G18 XZ, Plane Designation
G19 YZ, Plane Designation
TOOL RADIUS COMPENSATION
*G40 Cutter Comp. OFF/CANCEL
G41 Cutter Comp. LEFT, Left of Contour
G42 Cutter Comp. RIGHT, Right of Contour
*G44 Cutter Comp. Normal Feedrate
G45 Cutter Comp. Constant SFM
G48 Corner Rounding with Cutter Comp. OFF
*G49 Corner Rounding with Cutter Comp. ON
COORDINATE TRANSFORMATIONS
*G30 Mirror Image OFF/CANCEL
G31 Mirror Image X
G32 Mirror Image Y
*G72 Transformation OFF/CANCEL
G73 Transformation, Scaling or Rotation
MILLING CYCLES
G77 Zig-Zag
G78 Rectangular Pocket
G79 Circular Bore
G170 Outside Frame
G171 Inside Frame
G172 Pocket Frame
G173 Outside Face
G174 Inside Face
G175 Outside Circle
G176 Inside Circle
G177 Pocket Circle
G179 Slot
DRILLING CYCLES
*G80 Drill Cycle OFF/CANCEL
G81 Drill (Feed In, Rapid Out)
G82 Spot Face (Feed In, Dwell, Rapid Out)
G83 Deep Hole (Peck, Rapid Out)
G84 Tap (Feed In, Feed Out)
G85 Bore (Feed In, Feed Out)
G86 Bore (Feed In, Orient Spindle, Rapid Out)
G87 Chip Break (Peck, Rapid Out)
G89 Bore (Feed In, Dwell, Feed Out)
PROGRAMMING CODE SUMMARY FOR MILLS
G-CODE (Preparatory) & M-CODE (Miscellaneous)
G-Code PREPARATORY FUNCTION G-Code PREPARATORY FUNCTION
DIMENSIONS
G70 Input in Inches
G71 Input in Millimeters
*G90 Absolute Programming
G91 Incremental Programming
FEEDRATE
*G94 Feedrate Per Minute Mode
G95 Feedrate Per Revolution (pitch) Mode
WORKSHIFTS
*G54 Default Fixture Offset UCS
G55 Additional Fixture Offset
G56 Additional Fixture Offset
G57 Additional Fixture Offset
G58 Additional Fixture Offset
G59 Additional Fixture Offset
G92 Permanent Datum Shift
*G96 CANCEL G97
G97 Temporary Datum Shift
Z-AXIS MULTI-HOLE ROW DRILLING CYCLES
*G180 Drill Cycle OFF/CANCEL
G181 Drill (Feed In, Rapid Out)
G182 Spot Face (Feed In, Dwell, Rapid Out)
G183 Deep Hole (Peck, Rapid Out)
G184 Tap (Feed In, Feed Out)
G185 Bore (Feed In, Feed Out)
G186 Bore (Feed In, Orient Spindle, Rapid Out)
G187 Chip Break (Peck, Rapid Out)
G189 Bore (Feed In, Dwell, Feed Out)
Z-AXIS FRAME OF HOLES DRILLING CYCLES
*G190 Drill Cycle OFF/CANCEL
G191 Drill (Feed In, Rapid Out)
G192 Spot Face (Feed In, Dwell, Rapid Out)
G193 Deep Hole (Peck, Rapid Out)
G194 Tap (Feed In, Feed Out)
G195 Bore (Feed In, Feed Out)
G196 Bore (Feed In, Orient Spindle, Rapid Out)
G197 Chip Break (Peck, Rapid Out)
G199 Bore (Feed In, Dwell, Feed Out)
1104-3287
G-Code PREPARATORY FUNCTION
DIGITIZING CYCLES (OPTIONAL SOFTWARE)
*G200 Digitizing Cycle OFF/CANCEL
G201 Basic - Digitize Points, Lines, Arcs
G202 Mesh - Digitize XY Mesh
G203 Z-Trace - Trace Z Normal
G204 XY-Trace - Trace XY Boundary
G205 Cross-Section - (Trace)
M0 Program STOP
M1 Optional Program STOP
M2 Program STOP & RESET
(i.e., End of Program, RESET to Top of Program)
M3 Turn Spindle ON CW
M4 Turn Spindle ON CCW
M5 Turn Spindle OFF (Stop)
M6 Tool Change
M7 Coolant, Mist (also turns ON the ‘Thru the Tool Coolant’ Option, if installed)
M8 Coolant, Flood
M9 Coolant, OFF
M19 Orient Spindle (VMC Only)
M20 Program STOP, GO to Clear Point
M21 Optional Program STOP, Go to Clear Point
M22 End of Program, RESET to Top of Program but First Go to Clear Point
M25 Z-Axis Home
M26 Tool Change, Go to Clear Point
M28 Cancel Rigid Tapping Mode (i.e., Puts System in Open Loop Mode, VMC’s Only)
M29 Enable Rigid Tapping Mode (VMC’s Only)
M30 End of Program, RESET to Top of Current Numbered Program Only (Useful with BOSS 8, 9 & 10)
M36 Chip Conveyor FORWARD (Optional Part, VMC’s Only)
M37 Chip Conveyor OFF (Optional Part, VMC’s Only)
M38 Chip Conveyor REVERSE (Optional Part, VMC’s Only)
M51 Advance Index Table
NOTES:
This table was prepared using current Bridgeport Machine’s Controls available as of 4/98.
Modal & Non-Modal are defined as follows:
• Modal type code functions will remain active or effective until another code from the same group is executed.
• Non-Modal type code functions are only active in the block of programming in which it is specified.
G-Code & M-Code functions are separated into groups of Modal & Non-Modal code types. Modal code
functions are shown in a regular font. Non-Modal code functions are shown in an Italic font.
* Denotes those G-Codes which are system defaults when the machine is first powered up or reset.
CW Clockwise Direction
CCW Counter-Clockwise Direction
UCS User Coordinate System
REMEMBER:
Only ONE (1) M-Code function can be used in a Part Program Block!
M-Code functions are NOT allowed in Canned Cycle Blocks!
PROGRAMMING CODE SUMMARY FOR MILLS (CONTINUED)
G-CODE (Preparatory) & M-CODE (Miscellaneous)
M-Code MISCELLANEOUS FUNCTION
1104-3287

Terry,
This looks like a machining center list. A lot of the M codes the EZTRAK cannot do. I believe that most of the G codes are valid. He really needs a book describing the particulars for each G code. I suggest a V2XT programming manual from machinemanuals.net. A lot of what the machine can do is dependent on the contents of the BMDC.BIN file, or what capabilities are loaded into the BMDC board. That is why I suggest the V2XT manual and not the machining center manual.

George

George, Terry,
Thanks for your help - I will be able to use some of this information. I went to machinemanuals and there is not a V2XT manual to be found. I did however, find a BOSS 9 Series I & II R2E4 Programming Manual, BOSS 10 V2E3 Programming Manual, and a Bridgeport EZTrak Operations & Programming Manual 5.00.21/5.68 software & up and was wondering if one of these would do, or if you know of another source for this manual? Thanks again for your help!
Ron

I have the V2XT manual in PDF.

Terry

What I gotta do ta get a copy?
TKS
Ron

Send me your email address.

TM

Jaguar,
I hate to do the "me too" thang.......but could you send the pdf my way too?
clark@redneckgateart.com
thanks,
clarko

Hi, could I beg a copy? Pleeaase...

chalpha@hotmail.com

Hey There!
I thought I might as well jump on the bandwagon and ask for a copy of the V2XT manual as well.
WINGO46@msn.com
Thankyou
Al

If you contact Hardinge or EMI, they should be able to provide you with a copy of EZTRAK Ver 6 user manual in PDF - Hardinge sold me a copy about a year or so ago. I have it here someplace but it is BIG and chokes many mail servers when sent via e-mail.

They may make you buy V6 software but it is a bit buggy.

The Ver 6 manual contains the G code that the "TRAK recognizes. It does appear to be mostly a copy and paste of other G codes from other machines with some do's and dont's.

As long as you start out simple, you can get the code to work. Add features as you go and fix stuff that hangs/crashes the machind (do aircuts when debugging).

We have G code that cuts masters written from these tables. The code ports almost exactly into a HAAS with only subtle changes for tool R&R.

I would love to get a copy of this PDF as well. We are using the version 7.0 Software (last EZtrak Version) I had to create a custom post processor for Surfcam Velocity. And would like to know some better do's and dont's. I have been wanting to incorporate Cutter Comp without having to repost a comp adjustment from Toolpath file (Making a new post) I would like to incorporate the machines Compensation, since it does not use a tool Offset Database.

Any tricks to this?

glenn.lacefieldplastic@gmail.com

I found Today that G98 Does Not work with Ver 7. Ez trak BMDC

I had used Surfcam to layout a repeating Pattern and then had multiple drill points in a canned cycle.

The error i received was "bad Sequence" I tracked it down to "G98" Removed all g98 calls and it worked.

Still modifying my post processor, but it is slowly getting better.

Now im trying to figure out how to create a method of doing cutter comp....