Need Help!- Programming Mills To Leave Stock On When Profiling?

[Eddie1962]

Hi, please could anyone advise me on the lines of program I need to add to leave stock on when profiling. I know it can be done by using cutter comp (D value) but I don't wish to do it this way. I know that it is possible to add it in in the program by using a small line of codes before the line that puts on the compensation (G41/G42 line). Say for instance I wish to go round a profile three times, leaving it 1.0mm plus, followed by 0.2mm plus, and finally size, (plus 0.00mm). When visiting another factory I saw them using this method and would like to implement it myself. It's an alternative to "lieing" to the control and using 3 different Dia offsets, (ie, D01, D11, D21). Any help gratefully recieved.
Mr. Eddie Robinson

[Andre' B]

What I have done is take the highest numbered offset and use it as a temp.

You will have to look in your manual and find what system variables are use to store the offsets, in different machines I have found them at #2001, #10001, and #13001 also depends on if you have type I or II offsets.

But it goes like this.

The setup person puts the offset for tool 1 in offset 1 but in the program I only use offset 1 to calculate the value to put in offset 200 and then I use 200 of machining. I tell the setup people that offset 200 is only for my use in the program.

D200 = D1 + 0.010
Do rough machining using D200 as the offset.
D200 = D1 + 0.001
Do semi finish pass using D200 as the offset.
D200 = D1
Do finish pass using D200 as the offset.

[PBMW]

You must not be using a cam system eh?
Just askin...

[gar]

080412-1942 EST USA

Eddie1962:

What do you mean you do not want to use cutter comp? What do you think G41 and G42 are?

To do what you are indicating you want to do you need to use cutter comp, either G41 or G42. These make use of the cutter diameter and offset the actual cutter path by 1/2 the tool diameter from the tool table. 3d surfacing is a whole different story because G41 or G42 only work in one plane. Thus, no way to determine the perpendicular distance to the surface tangent plane.

Effectively you have to lie to the control about the cutter diameter.

See the thread I created some time ago where I describe a means to adjust tool diameter from the program.
http://www.cnczone.com/forums/showthread.php?t=12545

.

[Andre' B]

Originally Posted by PBMW You must not be using a cam system eh? Just askin...

But who are you asking?

I can't see who you are looking at thru the monitor.

[PBMW]

I guess either of you.
Why would you use three or four offsets to do a profile?
Tell the cam system to make a rough and a finish pass or five rough passes and a finish pass and three spring passes in about 30 seconds. post it and done.
I'm not getting down on anyone. I just never heard of anyone doing that and it seems quite inefficient to me. That would be pretty indicative of someone not using a cam system.

[Andre' B]

Sometimes loading up the CAD and CAM software is more trouble then just writing the program in a text editor.

But mostly I do it when I want the machine operator to be able to optimize the stepover size, stock left for finishing, etc. at the machine.
Otherwise we would need a computer and a seat of CAD/CAM software out on the floor for each or at lease every 2 or 3 machines.

[PBMW]

Interesting
I have five machines and am in thee midst of buying two more.
I have two seats of Mastercam and one of Gibbs
I worked in a proto shop where each guy programmed their own jobs, Usually, you can do it MUCH faster in the cam system.
If you have just one seat and it's not out on the shop floor, that's another issue, but cam is faster by far.
Also MUCH less chance of a mistake that will crash your machine causing repair and an upset schedule

[shawncnelson]

I've had lots of succes using G10. Put it at the beginning of you contour routine. Like this:

G91 G10 L13 P12 R.02
G90

That will leave .02 material. and only use one offset. This is written for Tool#12.