VF0: is there a way to use T7 but H8 length offset

[fattybean]

I am using an end mill for one side of a job I want to flip the part over and use that same mill for 2 more pockets but when flipped the Z zero is higher.

So I tried to use a different length offset, tool 7 with the H27 offset, but the mill alarms telling the T7 has to be the same as the H number.

Is something turned off that I can turn on or a code that I can add to the program?

[ckirchen]

Setting 15, H & T Agreement, allows you to use a different tool offset number.

Why not use two different work offsets? G54 for the first side and G55 for the second side. The X/Y registers would be identical between the two offsets and the Z registers would reflect the difference in thickness.

It's a lot safer than turning off setting 15.

[Geof]

I think it is risky turning off H and T agreement and it is not needed, use G52.

G52 Z-n.n will move the Z axis down by the distance n.n so you just put this ahead of the operations the tool performs on the flipped part.

G52 Z0. cancels any entry.

[fuzzyracing1967]

If you want to stay safe and not turn off setting 15 and for what ever reason you don't want to use G54 and G55 or for that matter G52 you can use G10.What G10 does is call out the offset in the program itself,this can be handy when useing a cutter on a arbor and needing to cut with both the top and bottom of the cutter at differant z's.Just a nother way to skin that cat

[fattybean]

Originally Posted by ckirchen Setting 15, H & T Agreement, allows you to use a different tool offset number. Why not use two different work offsets? G54 for the first side and G55 for the second side. The X/Y registers would be identical between the two offsets and the Z registers would reflect the difference in thickness. It's a lot safer than turning off setting 15.

I am using G54 and G55, the 2 are different because I want to stay on the same corner when flipped, they are 2 bearing pockets that have to be aligned, my X's are the same but the Y is flipped to the other side when I turn over the part.

I am new to Haas and mills, where is this setting 15? Is it only unsafe in an idiot proofing manner or for some other reason. I am very careful when proving out a program.

When you talk about the Z registers do you mean the Z"area" that is blank after the X and Y in the work offsets, which would offset all tools + or - Z? I need just the one tool, and the part has different surface heights.

I am accustomed to using this with lathes where I have a tool call of say T070707 or T0707 where I can adjust for conditions easily, I thought this would be the simplest fix for what I needed.

The parts are a prototype that I am trying different methods of operation and the boss "needed" it ASAP so flexibility and ease are my needs, I want to be able to touch off the tool and run it how ever I am holding it or no matter the extrusion thickness variances. I didn't want to use the G52 because the material varies, I wanted to touch off on the actual surface to be cut.

All suggestions are appreciated, they may not work in this case but will help on another.

[HuFlungDung]

It really doesn't matter that a value in G55 Z would shift all the other tools. If you're not calling any but one, that is all that matters. The rest are irrelevant. Or you could use G56 Z if you want for that operation.

[mactec54]

Hi Fattybean

I do what you are doing with no problem on a lot of jobs that you flip you can do what
the other post have said or just us a G54 for one side & a G55 for the other

2 Programs same tools set your tools to the part that will be the highest point/side which is the fliped side in your case this could be your G55 program then for the other side the tool or tools will have a longer programmed Z depth in your program this is your G54 Program this is better & safer than messing with the control

[fattybean]

Ok, I got it, pardon my density. So you're saying use G54 for side one, G55 for side 2, and for the 1 tool that is used on both side use G56 with an altered Z to make up the difference in height when the part is flipped.

Thanks for the help.

[mactec54]

Hi fattybean

No that is not right G54 is one program & G55 is the other that is all you need (No G56 Needed that will not work)

Touch of your tool to the highest point on your part this will be you fliped side let this be say G55 T7 programed Z-.5 now this tool #7 will go & cut .5 off your part

Now flip your part this this will be the lowest side of your part or were you will start from program with a G54 T7 your Z depth is set to the depth that you need in your program
it may be any number to get the job done like Z-1.5 ( You do not touch the tool off in this program you just put the Z depth that you need in your program to get the job done)

This G54 program my only take .5 off the job as well but by fliping your part you need more Z movement it's just what ever you put in your program to get the job done

Just remember the tool 7 was set to the highest side any other settings for your Z movement is all done in your programs

[Malish]

G54 & G55 (as well as G56 to G59 on the Hass Controller) are "work" coordinate systems. This is the X-Zero, Y-Zero, & Z-Zero that the controler will use when running that code. Normally if your not moving a part you will just use a G54 in your program once. But in this case you program the top with while using G54, then right before your code for the 2nd side you would insert a G55. So then it would use the G55 X-Zero, Y-Zero, & Z-Zero, which would be set to the the fliped side cornner and the new Z height.

You should not turn off the H and T agreement as a simple typo could crash the machine very easlily.

[HuFlungDung]

One point which may be missing in this discussion, and it has to do with the reference surface you are setting your tools off of.

If you have two tool sets, with one common tool shared between the sets, then you must set all the tools off one reference, and not use two references. I'm not clear on how you set the tools up originally. This way, it is safe to move either tool set up or down with the workshift and maintain the correct relationship, since you can only have one tool length measurement.