How to make programming easier for newb on old machine.

jamscal · Aug 8, 2017

What technology (programs) can I use to make programming simple jobs on my old machine easier?

Kiwa Excel Center 4 with Fanuc 3M C controller. Circa 1984

It has a db-25 female plug but there is no drip-feed possibility.

"Someone" says I can still upload small programs via a cable from a computer. Can I?

My problem is I'm a fabricator and not a machinist. I'd like to use a computer to create code for me but don't know where to start.

We currently only need to make simple programs (drilling hole patterns in tube, slotting tube, etc.) but I'd like to avoid pecking in one line at a time if I can avoid it.

(Yes I need to understand the basics more, I do have a cnc plasma cutter running Bobcad, sheetcam and Mach3)

cwtoyota · Aug 8, 2017

jamscal said:
What technology (programs) can I use to make programming simple jobs on my old machine easier?

Kiwa Excel Center 4 with Fanuc 3M C controller. Circa 1984

It has a db-25 female plug but there is no drip-feed possibility.

"Someone" says I can still upload small programs via a cable from a computer. Can I?

My problem is I'm a fabricator and not a machinist. I'd like to use a computer to create code for me but don't know where to start.

We currently only need to make simple programs (drilling hole patterns in tube, slotting tube, etc.) but I'd like to avoid pecking in one line at a time if I can avoid it.

(Yes I need to understand the basics more, I do have a cnc plasma cutter running Bobcad, sheetcam and Mach3)

I still do nearly 100% of my programming using Windows Notepad, or on the front panel of my mill (Fanuc 11M).
I've never run Fanuc older than 6M, but I'm sure you can connect a PC serial port (RS232) to your machine.
Do a little research on setting up the port (you may have to adjust or find a couple parameters).
After that, you need a computer with a serial port. In my case, my laptop doesn't have a serial port, so I use the GUC232 USB to Serial adapter from IOGEAR. Once you get the right driver, that IO Gear brand unit works perfectly. STAY AWAY FROM THE CHEAP CHINESE USB/SERIAL ADAPTERS!

There are plenty of things written, around the web on getting the machine ready for RS232 and how to wire it up.

Next: Even if you plan to purchase some software, you should learn how a program is properly written and how YOUR machine works with programs. On these older machines, you just about cannot run them efficiently without a clear understanding of how NC operates.

-Learn the coordinate systems, work offsets and how to use them. (This is either G52 & G54 - G59, G92, etc.)
-Learn the tool offsets and how to use them with the available coordinate systems.

Your old machine will have very limited memory space. The problem with most CAM software is that it will create a large file. You may have to split large programs for complex parts into several operations and load each program one at a time. The RS232 connection will allow you to drip-feed programs. "drip feeding" is the term used to describe sending the machine a few blocks of code at a time, on demand, rather than sending the whole program before starting the cycle. This does tie up a computer, requiring it to be connected to the machine to run those longer programs.

Learn as much as you can while you search for software to take the programming load off of you.
I still do it by hand because I haven't found a suitable solution yet, although I'm learning Solidworks through my engineering courses in college right now.

litlerob1 · Aug 8, 2017

cwtoyota said:
I still do nearly 100% of my programming using Windows Notepad, or on the front panel of my mill (Fanuc 11M).
I've never run Fanuc older than 6M,

Actually the 3 is newer than the 6, I know it's stupid but a fun fact anyway right? I don't mind punching in basic programs into the control, so long as the interface is user friendly. Fansuc is notoriously NOT user friendly for that specifically. They were not designed with that in mind, PARTICULARLY the older controls.

OP you have bobcad, I know nothing about the platform so forgive my ignorance. How many machine definitions files do you have? Obviously you have plasma, do you have 3 axe Mill? If you do, then generate the code there and send it VIA RS-232, it will take some time setting up handshaking, but it's been done 1000000000000000 times at least.

If Bobcad has no Mill suite, write the program on a word processor, save as a text document and send it the same way (RS-232), I personally would avoid writing programs at that control to the extent of quitting a job. (shift, EOB, Enter, where's the fucking Q?)

R

deadlykitten · Aug 8, 2017

hy jamscal

you know those books, how to become a plane driver in 24 hours ? here, check this quick guide :

... learn specific for each machine - 1 hour

... configure a software to output code coresponding to those specifics - 1 hour

... build conections with cncs - 1 hour

... replace controller, so to suit your needs - no time recomandation

one way or another, all those listed above are requirments ( except for the last one )

jamscal said:
My problem is I'm a fabricator and not a machinist. I'd like to use a computer to create code for me but don't know where to start

... find a guy that can edit the output of your CAM, for the [ Kiwa Excel Center 4 with Fanuc 3M C controller. Circa 1984 ] and the [ plasma ]
... if he know postprocesor edit, than he will do it without questions

... i can recomand you 2 such guys, but ...

jamscal said:
"Someone" says I can still upload small programs via a cable from a computer. Can I?

find this guy / someone that will make this conection for you

i would try at local automatization shops, asking in left&right for skilled eletronic guys, etc ... i can recomand you 3 such guys, but ...

cwtoyota · Aug 9, 2017

litlerob1 said:
Actually the 3 is newer than the 6, I know it's stupid but a fun fact anyway right? I don't mind punching in basic programs into the control, so long as the interface is user friendly. Fansuc is notoriously NOT user friendly for that specifically. They were not designed with that in mind, PARTICULARLY the older controls.

OP you have bobcad, I know nothing about the platform so forgive my ignorance. How many machine definitions files do you have? Obviously you have plasma, do you have 3 axe Mill? If you do, then generate the code there and send it VIA RS-232, it will take some time setting up handshaking, but it's been done 1000000000000000 times at least.

If Bobcad has no Mill suite, write the program on a word processor, save as a text document and send it the same way (RS-232), I personally would avoid writing programs at that control to the extent of quitting a job. (shift, EOB, Enter, where's the fucking Q?)

R

I agree about the front panel and ease of use on old Fanuc. Terrible. I use macros and templates to do most of my programming. With a good set of templates for your machine, all you really have to do is set up the tool changes and tool-paths. I use a script I wrote for generating tool-paths (G1, G2, G3, etc).

OP, I HIGHLY suggest using templates if you program in a word-processor or notepad. Create templates as you learn and master operation types. Search the web or I can send you some of mine to try for canned cycles. Here's an example of one of my most used templates for making holes.:

Drilling:
1) Cut and paste this code into your program within notepad.
2) Press CTRL H keys simultaneously to bring up the find & replace dialogue.
replace bb with your tool number for drilling.
3) Change the Z value to your depth of cut, R value to your clearance plane, F to your feed rate,
set your S spindle speed. (note the default z depth is shallow because sometimes you'll forget to change it.)
4) replace the X and Y values with your hole coordinates and decide if you need G90 or G91
5) scan with your eyes for lower case letters, or use the find/replace dialogue in notepad. (Lower case is an item you've overlooked)

Code:

G90G0	X		Y		Tbb
M6
(Tbb 0.0000" DIA DRILL HSS)
M1
(SET TOOL HEIGHT OFFSET Hbb)
(Tbb 0.0000" DIA DRILL HSS)
G43HbbZ.1S1000M13
G99G81Z-.05R.1F5.

xy
xy
xy
xy
xy

G98
G80G90
G0Z1.M9
M5

Here's a macro that I wrote for tapping a hole at the current position. If you have the memory space to keep one like this around, macro option and a tension tapping tool, a small program like this can save you a lot of time when you're doing a one-off job or writing a larger program with a lot of features by hand. More importantly, it can save you a lot of head-scratching and costly mistakes.

Code:

%
O9014(TENSION/COMPRESSION TAP G104)
(2017 C.WILKINSON)
(SET PERAMETER 7054 TO 104)
(TO ACTIVATE G-CODE G104)
(USAGE: G104 Z-.75 S100 T18)
(Z = DEPTH, INCREMENTAL)
(S = SPINDLE SPEED RPM)
(T = THREADS PER INCH)
(-OPTIONAL, R-PLANE)
(R = R-PLANE, INCREMENTAL)
(FEEDRATE IS CALCULATED)
(G90/G91 MODE IS PRESERVED)
(#4003 IS MEM ADDRESS: G90/G91)
#33=#4003
G91(WE NEED ABSOLUTE)
IF[#19EQ#0]GOTO1019
IF[#20EQ#0]GOTO1020
IF[#26EQ#0]GOTO1026
IF[#18NE#0]GOTO180
N180#18=0(NO R-PLANE SPECIFIED)
N200(DO MATH)
#32=#19/#20
N300(TAP A HOLE)
G91S#19M13;
G99G84Z#26R#18F#32P0
G98M9
G80M5
N1000(RETURN TO PARENT PROG)
IF[#33EQ90]GOTO1090
IF[#33EQ91]GOTO1091
(SHOULD NEVER GET HERE)
(SOMETHING WENT WRONG)
(WITH THE COORDINATE SYSTEM)
#3000=1(CANNOT SET ABS OR INC)
G0T01100
N1019
#3000=19(SPINDLE SPEED, S REQUIRED)
G0T01100
N1020
#3000=20(THREADS PER IN, T REQUIRED)
G0T01100
N1026
#3000=26(THREAD DEPTH, Z REQUIRED)
G0T01100
N1090G90(SET ABSOLUTE)
GOTO1100
N1091G91(SET INCREMENTAL)
GOTO1100
N1100(RETURN)
M99
%

CarbideBob · Aug 9, 2017

I think the starting point is notepad and a comm program.
The playing with the wires and protocol takes someone familiar with RS-232C and maybe a breakout box.
Bob

angelw · Aug 9, 2017

jamscal said:
What technology (programs) can I use to make programming simple jobs on my old machine easier?

Kiwa Excel Center 4 with Fanuc 3M C controller. Circa 1984

It has a db-25 female plug but there is no drip-feed possibility.

"Someone" says I can still upload small programs via a cable from a computer. Can I?

Hello jamscal,
Following is the cable pin-out and parameter setting to establish communication between the machine's control and an external PC.

Loop-back Null Modem Cable Connection
Machine Side -------------------------- PC Side
DB25 Male Connector ------------- DB9 Female Connector
1 --- Shield Trace ---------------------- Not Connected
2 ------------------------------------------------- 2
3 ------------------------------------------------- 3
4
| Bridged
5

6
|
8 All Bridged
|
20

7 ------------------------------------------------- 5

Machine Control Parameters
Parameter
0014
Bit 0 = 0
Bit 2 = 0
Bit 7 = 1
Parameter
0069 = 4800

Control Setting Page Settings
ISO Format = 1
I/O Device = 1

The above parameter settings are for I/O Device 1. If Device 0 is set in Setting Page, parameters 0005 and 0068 are used instead of 0014 and 0069

PC Transfer Software Configuration
Handshake Method = Xon Xoff (Software Handshake)
Data Bits = 7
Stop Bits = 2
Parity Bit = Even
Baud Rate = 4800

Regards,

Bill

Search

Largest Manufacturing Technology Community on the Web

Search

How to make programming easier for newb on old machine.

jamscal

Stainless

cwtoyota

Cast Iron

litlerob1

Diamond

deadlykitten

Banned

cwtoyota

Cast Iron

CarbideBob

Diamond

angelw

Diamond

Similar threads