having trouble with subprogram

[dshowald]

i have an 8x8x1" piece of steel that needs ends milled.instead of doing an outside rectangular cut i just want to do a line like im just milling the ends in a bridgeport mill.i have about .5 to come off.i want to step it over about.1 without me going back and changing cutter comp.i know i need to write a subprogram with .1 incremental moves but having trouble.any help please??

[LYN BYRD]

Are You Programming In The Conversational Mode?

[jpawelk]

How are you programming (conversational or text)? How far down would you like to go with each pass? Many questions to be answered in order to help you. If you would like, please email your situation to service@milltronics.net and we can further discuss your program.

[dshowald]

i am programming in conversational

[LYN BYRD]

If Your Machine Has A Z Axis, I Would Create A Start Mill Cycle And Set The Z To Make 4 Passes And Then Run A Clean-up Pass. With That Much Material To Remove, You Will Get Better Results Using The End Of The End Mill Rather Than The Side. Use The Side Of The End Mill For The Finish Cut.

[Farmers Machine]

Milltronics has a very simple sub program system on their mill controls.
The suggestion by Lyn Byrd is the most logical way to do the job, but there are cases where you must step over instead of stepping down. We will work with X 0 on the right side and Y 0 on the stationary jaw side. Convesational
Program set up page.
tool change page.
A position move to an X Y location to make the first cut.
something like X.5 Y.5
A position move to the Z cutting depth. We will stay at this depth for all moves.
Subs
Start subprogram and give a # like # 1
This is where you must be really careful.
Misc. arrow to the bottom and type G 91 Changes to incremental
go to Mill/Geometry/Line and fill in Y-8.5 Machining feed rate.
next move is clearance X.03 Machining feed rate.
Next move is a high feed rate back to the
start point in incremental. Y+8.5 about 100 IPM Be safe
Even though it is +8.5 it really takes
you back to Y.5 where you started.
next move is stepover amount
plus clearance. X-.1 -.03 For X-.130 Machining feed rate.
Subs
End Subroutine.
Misc. Arrow to the bottom line and type G 90 This will put the machine back into absolute.
Subs
Go subroutine/ Loops/ Fill in # for how many times to step over.
Teach the tool to Z 0
hand wheel up and remove the tool
Cycle start the job and make sure that all moves are in the propper sequence and location. When you are sure the machine will not be hurt and the part scrapped install the tool and cut chips.
There will be a need every now and then for a job like this. It works best for me to draw out the tool path on paper and think about the Incremental moves, from where I am now, how far in what direction do I go from here.
Good luck. The Farmer

[AMCjeepCJ]

Hey,

I've always meant to try this and always forget to... Has anyone ever programmed a straight line and used the Z passes and THEN rotated the whole thing 90 degrees around the Y axis?? It might make really short work of programming the steps in from the side. Like I said, I always forget about trying it but I bet it's SUPER easy once you try it a few times... If I remember, I'll try it in a few days when I get some extra time... (The plus side is it's only one extra screen in conversational but I think you'd adjust your cutter compensation via your "first Z depth", followed by your left over stock being taken out with your Z increment)

[AMCjeepCJ]

Nope, it didn't work, lol, maybe if you added a "text" editor rotation around the 'y axis', not a point ON the 'y axis' like conversational does...

[LJ48]

Hi Guys
1st for Farmer when you are talking about a sub program, are talking about a whole new program or is there a actual place for a "subprogram". I have done this by using 2 small programs and the program I am using to cut part. What they use is the "set flz" to set a new "x" zero point, I have it written down on how I did it but can't find it right now. I will find it clean it up a bit and repost it, maybe as a MS- Write program. What is nice about it is that it is all conver. and if you have a part stop when you run the second time the old "zero point will back up to where you did the first pcs.this was for a cent. V control

2nd for Jeep (sorry lazy typer) you might be able to do what you want with by adding "rotate" from the "spec" "F8" there is stuff like rotate, scale, set-flz. I have used rotate on a rect pocket I did a rect. pocket made sure it looked what i wanted then just added a rotate.

I used to have a Cent.V, but my Co. finaly got an up date to Cent. VII, real nice control . It seams with Milltronics controls If you think there is an easier way to do something , look around there probably is. I only use conver. Hate G-code!!!!!!!!!!
sorry to talk so much LJ48

[AMCjeepCJ]

Hiya LJ,

I have V and VII depending on which machine. I booted up the VM-22 and tried it in conversational, it didn't work since in conversational it is looking for a point to rotate the Z axis around, you do not have the option of rotating around ANY other axis. I do not understand however why it has a Z box to fill in?? This is misleading to me, it was because of the third box I thought it might be possible but I tried a few different configurations and no luck so far. If anyone can get it to work though, please post a copy of your conversational program, I'd really like to see it work!!

[AMCjeepCJ]

As far a sub programs go, this is how I normally do it. Seems to be the fastest way once you get reasonably proficient on the control. (Without using incremental that is...) I'd say it would take maybe 2-3 minutes to program. BTW, I wouldn't use incremental moves, I'd use 3 or 4 calls and then a floating zero to start my sub... (Hope that helps)

Here's an example:

I zero'd out on the lower right part of the part to side mill. This part is 4 inches wide in Y and we're taking .375" off on the right side in .125 increment passes with a .01 finish pass at a different RPM and feedrate.

Program 1 is simply...

1. Toolchange

2. POS X .25

3. Call Prgm 2

4. POS X .125

5. Call Prgm 2

6. POS X .01

7. Call Prgm 3

Program 2 is simply...

1. Floating Zero X=O

2. Start mill cycle (X=0 Y=4.25 and fill in all the other crap and turn cutter comp on to do one pass) (PS: The Y is at 4.25 to climb cut, if you have lots of backlash, start at Y=0 and move TO Y=4.25)

3. Line move Y=0

4. Mill end (auto)

(Turn all the last page to NO NO NO NO)

Program 3 is simply (copy Prgm 2 to Prgm 3 and change your feedrates and add a misc. command if you want to modify the RPM)

If you write that program once, you can use it forever by just reassigning the X and Y values for each job...

Stay away from incremental if you're not used to it. It's easy to do a Call loop too many times in the main program but if you do use inc., it might be a little shorter of a program but not very much much unless you had to do ten or more passes~

I try not to use incremental very often although it is handy once you get it down pat. However, this method is waaay simpler for the average Joe who isn't programming everyday...

Good luck...