Macros

[cncfreak]

Hi, I'd love to talk to people about Macros used in programming. I've created some of my own for use on a Haas VF-2. I have found little info in the web other than Haascnc.com and people that want to sell you something. It would be great to get something going here to share macros and come up with ideas for new macros.
Thanks

[MPE racing]

Hi CNCfreak, I've done some macro programming. Mostly I've used it for changing tool diameters between loops to create tapers. I've also written one that does pocketing.

Go to www.programmingunlimited.com
This is a pretty good site. I would suggest you buy the book off him.

[MachineSMM]

I have made a lot of Macros. Email me tomorrow and I can send you a whole bunch of them that I have made and gotten from other people.

Any questions in particular that I can help with. If there is anything that you do all of the time in your shop, you must make a macro for it. It can make your life much easier.

I use a Cad/Cam package called VX, www.vx.com. They have an internal macro language that I used to automate the programming fo some of are standard molds. It use to take about 2-4 hours to program these molds but now All you do is enter a couple of variables and presto the program is ready for the CNC.

Please fell free to contact me anytime

[hardmill]

Who said macro?
Cool, what do you got in mind?

[cncfreak]

Well I have two macros now one for face milling and one for side milling on a Haas mill. This mill is used in our Toolroom and we are always taking sawed stock and milling it square. When ever I write a cnc program I alway assume the stock is already milled to size and square. Becouse I never know what size of stock the toolmaker will grab. This way the toolmaker can grab any size stock they want and use the macros to quickly mill it to size and square. Then my Cad/Cam program will do the rest. I'm looking to do some macros on the Haas lathe but have found out that you cann't use macros in canned turnning cycles.

[cncfreak]

If anyone has found a good use for macros for a lathe, I would love to hear about it.

[Turbine]

I emailed ya a good un. I have more.

[Turbine]

Here's a mill one to blast a circle pocket without a start hole. It has slick helical motion. My favorite lathe one is in your email. (Sorry guys... It wouldn't be right for me to post that one here as I did not write it.)

• O9001
  (VERSION 1.1 - 2/17/03)
  (X=X CENTER)
  (Y=Y CENTER)
  (Z=FINAL DEPTH)
  (B=BORE DIAMETER)
  (C=CUTTER DIAMETER)
  (D=DIRECTION, 2 OR 3)
  (W=DEPTH PER PASS)
  (R=START PLANE OF MATERIAL)
  (F=FEED RATE)
  #30=#4001
  #31=#4003
  #32=#4109
  #33=#5043-#5083
  IF[#24EQ#0]THEN#24=#5041
  IF[#25EQ#0]THEN#25=#5042
  IF[#18EQ#0]THEN#18=#33
  IF[#9EQ#0]THEN#9=#32
  IF[#26EQ#0]OR[#2EQ#0]OR[#3EQ#0]OR[#7EQ#0]OR[#23EQ#0]THEN#3000=1(INSUFFICIENT INFORMATION SUPPLIED)
  IF[#23LE0]THEN#3000=1(ILLEGAL W SPECIFIED)
  IF[#2LE0]OR[#3LE0]THEN#3000=1(BOTH BORE AND CUTTER DIA MUST BE GREATER THAN ZERO)
  IF[#26GE#18]THEN#3000=1(DEPTH MUST BE LESS THAN START POINT)
  IF[#26GT[#18-#23]]THEN#3000=1(W VALUE TOO GREAT)
  IF[#3GE#2]THEN#3000=1(CUTTER CAN NOT BE BIGGER OR EQUAL TO BORE DIAMETER)
  IF[#7EQ2]OR[#7EQ3]GOTO5
  #3000=1(ILLEGAL DIRECTION SPECIFIED)
  N5#29=#2/2-#3/2
  G00G90X#24Y#25
  Z[#18+#23]
  #18=#18-#23
  G01G91X#29Z-#23F#9
  N10G#7X0.Y0.Z-#23I-#29J0.
  IF[#18EQ#26]GOTO15
  #18=#18-#23
  IF[#18GT#26]GOTO10
  #23=#18+#23-#26
  #18=#26
  GOTO10
  N15G#7X0.Y0.I-#29J0.
  G#7X-#29Y0.I-[#29/2]J0.
  G00G90Z#33
  G#30G#31F#32
  M99

[cncfreak]

Hay, Turbine I didn't recieve your e-mail.
and I cann't e-mail you through this board.
Thanks.

[Turbine]

freak,
The program is too long.
I could not PM it either. There is a 3000 char. limit.
Check your PM anyways I sent you my email.

[ty1295]

If anyone has found a good use for macros for a lathe, I would love to hear about it.

I have developed at work a macro for turning aerospace piston rings. Basically you give info on raw material, tooling, speeds/feeds, and finshed part size. Macro then machines rings, keeping both turretts (4 axis lathe) in sync.

I also have sub running that double check operator has not changed chuck barriers or X offsets on machine, and either automatically fixes them, or throw up an alarm.

Program is now 4 subs, and the main totalling 6-7 pages. In the 2 + years it has been used, I bet it has machined close to a 1/2 million rings. Has saved MANY hours, and prevented several crashes.

I can't post the program, since it belongs to work, but I can guide in developing yours.

All mine was done on an Okuma, but other controls all operate similar.

I find myself using small macros even when doing simple 1 off parts. For example I tend to leave my math in the programs.

(G1 X=3.0+.05)

Helps me when I come back later, remeber where the numbers are coming from.

[nocamhere]

Has anyone written a macro to repeat a subprogram x number of times? We do alot of repeated work at our shop. we'll load a large piece of stock into the machine and machine a profile into the stock. We then repeat the profile over in x...then the whole row down in y. we'll get like 8 parts froma single piece of stock....


has anyone written a macro to write the repeats for this? I've tried, but i keep getting illegal macro operation errors (fanuc 0i-ma)