Issues with transferring cam programs to MX2 prototrak.

I have an MX2 A.G.E. bed mill. I inherited from my uncle last year. I use it as a hobby in my garage. I'm familiar with the machine and the capabilities of it. I have Mastercam and Millwrite available to me to use at anytime. Basically, what I'm getting at is I can't get the laptop to connect to the rs232 to have the program transferred properly. I'm using a usb to rs232 db25 connector with a null modem adadpter from Cable 2 Go. It will transfer but 1 of 2 things will happen. With engraving, it will only repeat the first letter for the length of the program or only about 75% will be transferred. Also, I bought a 3.5 external floppy writer so I could transfer that way... it can't read ".cam" files through the mx2 floppy port. After discussing with SWI, it's an up gradable feature for $425 to get a 3.5 floppy with the "MX2e" boot up floppy. I will not pay that much for 24 year old technology for something I don't make money with. If you have any tips or tricks please let me know. Thank you in advanced.

LJMason13 said:

I have an MX2 A.G.E. bed mill. I inherited from my uncle last year. I use it as a hobby in my garage. I'm familiar with the machine and the capabilities of it. I have Mastercam and Millwrite available to me to use at anytime. Basically, what I'm getting at is I can't get the laptop to connect to the rs232 to have the program transferred properly. I'm using a usb to rs232 db25 connector with a null modem adadpter from Cable 2 Go. It will transfer but 1 of 2 things will happen. With engraving, it will only repeat the first letter for the length of the program or only about 75% will be transferred. Also, I bought a 3.5 external floppy writer so I could transfer that way... it can't read ".cam" files through the mx2 floppy port. After discussing with SWI, it's an up gradable feature for $425 to get a 3.5 floppy with the "MX2e" boot up floppy. I will not pay that much for 24 year old technology for something I don't make money with. If you have any tips or tricks please let me know. Thank you in advanced.

Click to expand...

.
must be setup on computer
4800, e, 7, 1
.
if you use different serial port setting it will not transfer file
.
Gcode must be on every line
Gcode must have space between them
End of Block character must be semicolon (this often will stop program at 1st line cause stuck and will not read next line, end of block is end of line) so adding semi colon to each end of line is needed if post processor does not do it. i have change it in mastercam to add semi colon automatically to each end of line. takes time figuring it out. it is a mastercam thing
.
it prefers prototrak gcode but often Fanuc 6 gcode it will read and translate but will need testing
.
Fanuc 6 is 2 axis it does not see Z and thus no Z axis will be translated
.
MX2 and AGE2 are different. some AGE will translate Fanuc much better than earlier MX2 or Prototrak Plus models
.
file size limit is a little over 200 lines
.
i have used edytornc software to file transfer. you will need to check and change default settings to 4800, e, 7, 1
.
mastercam has file editors that will file transfer too but again you need to check default settings
.
EdytorNC download | SourceForge.net

often letter and numbers can be in millwrite pick font 2 axis standard
.
it lessens Z axis moves and uses more arcs not many little lines to make a arc. this reduces file size or number of program lines considerably
.
best to keep it at 200 lines or less the program length.
.
i often had to edit z axis moves as early prototraks do not see Z so a
XYZ move where X and Y stay the same it will stop as it does not see Z and sees a line with no change in X and Y
.
either edit program manually or program a helix as starting move thus when it fails to see Z it will see a X and Y change
.
editing often needed as you have to determine when to stop to manually raise and lower Z
CR-
when it sees it stops and waits for go button push. you add where you want to adjust Z manually
.
incremental and absolute (big difference) Begin End (big difference)
XB1.0000A
XE1.0000I
takes time to learn to read SWI or Southwest Industries gcode
arc center are incremental ( from end point to center) but opposite from fanuc incremental from start point to center
.
it will take Fanuc 6 (2 axis) gcode and translate to SWI gcode but again some editing is often needed
.
i made a tool holder to hold a sharpie marker to draw engraving on part before actual engraving. but MX2 and AGE2 should be able to draw on screen for you. none the less it helps to run program not cutting to check if program ok

forgot to mention
.
transfer Fanuc gcode to prototrak and then transfer back to computer to read and edit it as it will translate from Fanuc to SWI code (and translation often not perfect)
.
it does not directly use Fanuc gcode. it translates it to SWI gcode
,
seems complicated but i often wrote engraving in millwrite then engraved part and was done in 20 minutes. but not like you will engrave a book. usually only engrave one or 2 lines
.
engraving a ruler with lines and numbers was a lot of manual Z axis moves

DMF,
Thank you for the help. I'm still not having too much luck. Still the same issues. Haven't tried the EdytorNC yet either though. Some of the other people are saying it's my computer's operating system. I should be running something with XP. I think that's crap but I have an old tower I can try instead of my laptop's. That probably won't happen till the weekend though. Too cold in the garage for now. I'll be trying to change it to Fanuc 6 as well. It's becoming way to frustrating. I feel like it should just work because it is old tech.
Side note, on the controller is says "Proto trak MX2." On the name plate it says Trak TRM.
Do you have the MX2"e" software?
Thank you again for the info.

I have a real MX2e disk that I have no use for. Not a fake. Reach out to me if you are interested. endmill at maine.rr.com