| | |
As a new user to swiss I am constantly finding out how little I know. When a program works fine for say a double angle bur shape at one diameter, say .062 and I want to make a bigger diameter of say .1161 why can't I just leave program alone and input the new x and z measurements. This is a 2 turret citizen, and out of same diameter (.125) M2 stock.
There are ways to help you make quick changes like that, BUT, you have to write the program in a way that will allow you to change that way.
Macro programing for a "family" of parts is what you are looking for. You could set it up so you would go to a page under "Offsets" and enter the numbers that need to change. When you have written the program correctly, and have ALL the tools in the machine, it would take seconds to switch to a PROVEN part.
post your code and we can probably macro it out for you
Hi What I have is a bur that has angle at top and barrel sides. It worked for for a .2204 diameter but wgen I went to .2649 it is whacked out and I can never get the diameter as I need it, seems to stay at 3.12. I am using.3125 stock. code for front cutter is as follows:Originally Posted by cncswiss1
%
:1967
G58
G69
G50x-.15z-.10
/M52
M6
M3s3500
T1100
T2200
M10
M98P9021
G50u.184
G0z0x.413T11
G1x-.01F.0015
x0
z.1510x.2649
z.1346
x.343w.01F.003T00
G50u-.184
Have tried changing several things but diameter never changes.
%
:1967
G58
G69
G50x-.15z-.10
/M52
M6
M3s3500
T1100
T2200
M10
M98P9021
G50u.184
G0z0x.413T11
G1x-.01F.0015
x0
z.1510x.2649
z.1346 (this is actually moving back to z.1346 from z.151)(use W.1346 instead, incremental .134 more down the part)
x.343w.01F.003T00
G50u-.184
been a long tome since i messed with an F but this may do the trick
#500=.151 (BURR DIAMETER)
#501=41.0 (TIP ANGLE)
#502=.2856 (OAL)
G50u.184
G0z0x[#814+.1]T11 (OLD MEMORY THAT#814 IS STOCK DIA ON F?)
G1x-.05F.0015 (FACE WAY PAST CENTER)
X0 (USING A SHARP CORNER TOOL? MAY NEED TO BE X-)
x[#500] A[#501] (the a command for angle option is active right?)
Z[#502]
X[#814-.05] (.050 UNDER STOCK DIAMETER)
W.025 U.05 (.025 CHAMER TO STOCK DIAMETERTO REMOVE BURR ON BAR)
W.03 (WIPE OFF BURR TO BE SURE NO STICK IN GB)
G0 X[#814+.1] T0
G50u-.184
if your A angle option is not active we can substitute this line
x[#500] w[[#500-/2]/TAN[#501] ] (SOH CAH TOA BABY!)
I don't think his F20 has Macro programing. It is a 6T control. Plus Macro programing can confuse someone not ready for it. Learn the basics 1st. I don't teach macro until I am sure the person has a complete understanding of regular programing.
One might consider that macro-programming is regular. I don't teach people to program if they can't grasp the macro end of things. It can be used to really do some great things like making its own offsets after it probes itself. I haven't seen any bad advice from Cogsman yet. Seems to deal out some pretty good info. "x[#500] w[[#500-/2]/TAN[#501] ] (SOH CAH TOA BABY!) " I think this might alarm out for having the -/. But it is very nice to see others that use SOH CAH TOA!!! Thanx!
Yes , I agree macros are very useful. I have been programing macros on Citizen machine for 17 years and was taught by an expert in them at Citizen, when I worked for them. I don't think the F20 6T has macros so here you try to get someone to program a machine that may not have macros using macros the guy probably does not understand. Also I find most new guys don't know trig that well and you want to teach them how to use it in a macro?
Plus you are using #814 Which is a Machine Data Page # AKA "MC Data Page" from a L,M.C,E series. The F never had a data page, hence no #800"s ever!
been a long tome since i messed with an F but this may do the trick
#500=.151 (BURR DIAMETER)
#501=41.0 (TIP ANGLE)
#502=.2856 (OAL)
G50u.184
G0z0x[#814+.1]T11 (OLD MEMORY THAT#814 IS STOCK DIA ON F?)
G1x-.05F.0015 (FACE WAY PAST CENTER)
X0 (USING A SHARP CORNER TOOL? MAY NEED TO BE X-)
x[#500] A[#501] (the a command for angle option is active right?)
Z[#502]
X[#814-.05] (.050 UNDER STOCK DIAMETER)
W.025 U.05 (.025 CHAMER TO STOCK DIAMETERTO REMOVE BURR ON BAR)
W.03 (WIPE OFF BURR TO BE SURE NO STICK IN GB)
G0 X[#814+.1] T0
G50u-.184
if your A angle option is not active we can substitute this line
x[#500] w[[#500-/2]/TAN[#501] ] (SOH CAH TOA BABY!)
Last edited by Chuckforce; 03-20-2008 at 07:34 AM.
I did not post a program for anyone to use as i do not know all the controlers citizen uses. If he does not have macros, somebody got cheap and screwed this guy. My point was merely to say, that some people find it "normal" to use macros. I try to teach all that I know and as in depth as possible. I never worked for Citizen, but only had the opportunity to program a few of their machines. I find that teaching trig and macro programming will benefit me and the other guys to expand their capabilities and resumes. After all, trig is just a triangle. I was given all the training i have and am determined to give it all in return. I am sure you are the same way. I was not trying to offend you, and apologize if I did. I only know trig and macros. Never learned cad/cam post processing. Thank-you for your response. I will try to look into which controllers have which options.
No problem.
I think from the sounds of it he bought the machine used and is just getting started with it. Throwing macros at him will only confuse him, at this point and like I say the machine does not have them so he will feel even more frustrated when he can not get that to work.
His machine , F20 6T, is about 25 years old. Macros were mostly options back then and expensive at that.
Some may remember that the OT keypad did not have all the characters on it. You could not key in some macros variables but you could down load a macro them and run it.
Now most machines have them as standard.
I enjoy programing macros. We just did a piston shaft on a A20 VI that will run any length shaft, hell even up to 10' . It figures the number of full rechucks needed and calculates the length of the last one. We also incorporated a provision to run smaller shafts to reduce remnet lengths and save wasted stock.
Fun stuff. I look forward to helping out here also.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
