macro's

[Traceycnc300]

The company I work for bought a brand new Haas VF4.So we get 200hour of Macro's to try out.But I've never used them can someone show me where I can find a use for this feature.I've heard its some cool sh$$ but I can't see how its any better than regular G coding.Can someone shed some light on this for me. Thanks Tracey

[miljnor]

The biggest advantage of macros is that you can make whole programs that can take care of a class of parts. Within each class of parts, if the only change is size, then you can make all the changes thru variables.

Macros are very useful but mainly it depends on your programming style. If you have high-end cad and/or do 1 off parts you might not see the advantage.

But if you hand code allot or like to make little programs that fit a variety of needs then macros are indispensable.

[gar]

060402-2101 EST USA

Traceycnc300:

miljnor has given you some good perspective.

I will add the following:

You can do logic, math, and trig functions. You can easily pass parameters to subroutines. DPRNT is available which allows you to output data to the COM 1 serial port. You can create counters for special functions. You can easily do step and repeat functions, even with varying increments. You can write a program that will step and repeat for a variable number of steps, and do it efficiently without a lot of tool changes. You can access timers and operate on the values.

I have a standard tool change subroutine that can greatly reduce errors of hand coding. Also standard subroutines for collecting timing information from within a machine cycle.

The DPRNT function along with external equipment can provide a means to do special functions.

Scaling and rotation is another very useful option, but on our machines lacks independent scaling of each axis.

.

[Geof]

If you have not turned the 200 hour Macro trial on I suggest don't do it yet. You cannot turn it off and it will be a waste if you burn up all 200 hours on the early part of a learning curve. Find out what macros can do, get some samples and then when you are set turn on the trial.

[Traceycnc300]

Thanks guys.I am going to wait till I get better understanding before I activate the function.But I am interested so any examples would be apreciated.Then if I can show the boss man where it is usefull I'll try to get him to buy the option.I've read a little about it in the Haas manual but find it to be pretty vage.I've been programing by hand for several year and we also have acouple other good programmers but none of us have used macro's.So were very interested.

[gar]

060403-0631 EST USA

Traceycnc300:

Following is a thread I started on a Tool Change Macro:

http://www.cnczone.com/forums/showth...l+change+macro



And at some time you might want to study this thread:

http://www.cnczone.com/forums/showth...ighlight=dprnt

.

[Wiseco]

Originally Posted by Geof If you have not turned the 200 hour Macro trial on I suggest don't do it yet. You cannot turn it off and it will be a waste if you burn up all 200 hours on the early part of a learning curve. Find out what macros can do, get some samples and then when you are set turn on the trial.

You can turn off a trial that's been activated. Something you must not forget after turning a trial off is to cycle the power (power off, then power on). I've used the trial for rigid tapping and I turned it off after using it so this way, I'm not trowing away the rest of the 200hrs.

But I agree with you. If you don't really need it, don't activate it. This way, you'll be sure to not forget to turn it off.

[JPMach]

One of the easiest things you can do with macros is run several parts on the table. Simply program each part as you normally would with a different fixture offset for each. Then change the M30 at the end of each program to M99 and right one more small little program. Lets say you have three parts on table with programs O100 through O102 then make a program like this

O105
G65 P100
G65 P101
G65 P102
M30

The if you get more in depth on macros, say you wan to run two of part O101 on the table and only one each of the others. Then you simply need to make the fixture offset in the program for O101 a variable (say #100 use an empty one)and then your program would look something like this

O105
G65 P100
G65 P101 #100=56
G65 P101 #100=57
G65 P102
M30

Don't quote me exactly but that is close. In school I went above what the teacher new and wrote a parametric (read macro) progam for a part that we ran on an old BP and for a test another student did the same part by cam. I believe the cam program was around 8 pages of code or so and the program I made was a page and a half and was still easily adjustable for different size parts or diferent number of bolt holes.

JP

[JPMach]

Another way to look at things is that all canned cycles like drill cycles are esentially macros with variable arguments. They just happen to be built in.

JP

[Traceycnc300]

Thanks gent's thats the kind of info I was looking for.It's also nice to know it can be turned off to conserve.

[miljnor]

it Cant be turned off once turned on!!!!!

edit:
of course I didnt' see the other post on cycling the power so... of course ignore my ignorant remark!!!

[Stu_M3]

I use macros for milling angles on blocks at any rotation or location all i have to do is specify the position in (xy), rotation, depth, angle, length, peck, finishing peck, the macro does the rest.I have a few others for helical milling bosses, corner radii on blocks, pockets and rectangular profiles, All of them have protection against the user entering wrong data. Macros are really good when you do a lot of the same sort of operations and it saves using cad/cam to generate simple toolpaths.