ATC tool length problem

[leix_99]

Hi everyone, a couple of days ago i started playing with. 1996 vf2 in my dad's job, i have no experience at all but i started milling pu foam, i'm able to run entire programs made with rhinocam and the haas mm post, everything works like a charm except ATC. I can make a rough with a d10 flatmill but when an m6 triggers, machine ignores the tool length offset...
By now, i've been posting each op as an individual program and resetting the G54 z offset in every program to the desired tool length.

Can anyone tell me why the tool length is ignored by my machine?? I guess it's some mess with the G43? And also, what does the H letter mean in the code??

Thanks, i'm really excited to be able to run a machine that has been stopped for almost 10 years! And i want to get the maximum performance of it, any other advise or recendation?

[txcncman]

G43 Hxx calls the tool length offset saved in the tool table. Must be in the program to work.

[Machineit]

Hi everyone, a couple of days ago i started playing with. 1996 vf2 in my dad's job, i have no experience at all but i started milling pu foam, i'm able to run entire programs made with rhinocam and the haas mm post, everything works like a charm except ATC. I can make a rough with a d10 flatmill but when an m6 triggers, machine ignores the tool length offset...
By now, i've been posting each op as an individual program and resetting the G54 z offset in every program to the desired tool length.

Can anyone tell me why the tool length is ignored by my machine?? I guess it's some mess with the G43? And also, what does the H letter mean in the code??

Thanks, i'm really excited to be able to run a machine that has been stopped for almost 10 years! And i want to get the maximum performance of it, any other advise or recendation?

I would use your "TOOL" offsets for the tools for now and leave the (work offset) G54 Z length at zero. Set each tool at the top of the part using tool offsets #1 through whatever tool you use, on the tool offset page.

To call a tool change use the T2 MO6, but add the H02. The H is the code that calls up the tool offset for that particular tool. So a line for example would be:

T2 M06 H02;

I put my M08 after that when writing by hand so would be:


T2 M06 H02 M08;

Just remember that your G54, G55, G56 etc. are "WORK" offsets, and that you need to set "TOOLS" on the tool offset page.

Good luck and have fun. Remember that when checking out a programs, reducing your rapids to 5% or 25% is your friend. Crashes are no fun!!!

Mike

[leix_99]

Thanks machineit!

I'll try tomorrow a program that just switches various tools with a dial gauge, i guess i'll find the tool offset page in the haas panel and simply enter the length of the tool right?

Regarding the rapids, my dad said: if i ever hear or see the machine doing a rapid i'll cut your balls... so transfers aren't G00, just limited to 1000mm/min, as you said crashes are no fun.

[Machineit]

Thanks machineit!

I'll try tomorrow a program that just switches various tools with a dial gauge, i guess i'll find the tool offset page in the haas panel and simply enter the length of the tool right?

Regarding the rapids, my dad said: if i ever hear or see the machine doing a rapid i'll cut your balls... so transfers aren't G00, just limited to 1000mm/min, as you said crashes are no fun.

The length of the tool in these machines is relative to the top of the part you are cutting. I would not start with using a dial gauge. You have nothing to measure it comparatively to. Use the following procedure until you understand it better.

For example, you have a block of aluminum in the vise that is 3x3x3 inches. You are going to machine a pocket in the top of the block and you are going to use a rough and a finish tool.

Say your rough tool is a .5 inch endmill and your finish tool is a .125 inch endmill because you need that radius in the corners. You touch both tools #1 & #2 off of the top of the block of aluminum. To do that, you bring the first tool down to just over the block and switch to jog at .001 or .0001. You can then use a standard piece of paper to wiggle between to block and the tool as you come down to the part. When the tool touches the paper you will be about .003 to .004 inch above the part. Pull the paper out and go down .003" more. A standard post-it note is right at .004" thick and depending on how tight it feels when you first touch it, you can decide on .003 or .004 further. This method is what I have used for 20 years and will get you within .0005" or better.

At this time, go to the tool offset page and highlight tool #1's setting for (Length--Geometry). Press "Tool Offset Mesur" button, this will load the offset for tool #1 into the control. Then just push the "Next Tool" button and the machine will change to tool #2 and you will be ready to touch it off. The machine will still be in jog mode and will be in .01" mode and you just go back down and stop about the part and use th same procedure that you did for tool #1.

That same procedure is used for every tool you have, which could be 20 on that machine.

As for the part offset, decide where you wish to have zero on the block, one of the four corners or the center of the part and set that also using G54. I don't know what you use, but probably a edge finder with a .200" tip diameter. Whatever you use find your zero using that and then go to the part offset page where your G54, G55 etc. are. When you are on the exact location that you wish to use as zero, just set the X and the Y by hitting the "Part Offset" button.

DO NOT HIT THE "Z" offset under G54 etc.. That will add that length to every tool offset and it will crash. The Z offset is only for KNOWN tool lengths and KNOWN work piece heights. Like for shops that run the same programs very often and use the same tools that are of a known length.

So, your G54 should say something like X-10.5678 Y-6.9840 Z0.0 and your tools should say something like T1 -10.8635, T2 -12.7653.

At this point you are ready to run your program. Just make sure you cad system is set to the proper G54 location and that you are using the top of the part as Z zero for your program.

For testing your programs a good trick to use is to use the G54 Z setting to clear all your tools above the part for testing. For example, if one tool goes to Z-1.0 and another goes to Z-1.25 in your part, just setting the G54 Z setting to 1.26 will enable you to run the program without the tools ever touching the part. Remember to make the Z number a positive number, so do not put a - (minus) in front of it. To do this, just type your number in the Z column and hit F1. So, type 1.2 and hit F1.

After your test run, just go the the G54 Z and enter 0 and hit F1 again and you are back to normal setting and ready to run.

Have fun, sounds like your dad is pretty cool!

Grandpa Mike

[leix_99]

So if i directly know the real tool length, some of them were adjusted a loooong time ago, but still have a table with it's parameters, i can skip the paper procedure (in the future). Tomorrow i'll check the tools and try to set the offset as you explained and see if i sucess!
Thanks again for the reply, really really instructive!

[Machineit]

So if i directly know the real tool length, some of them were adjusted a loooong time ago, but still have a table with it's parameters, i can skip the paper procedure (in the future). Tomorrow i'll check the tools and try to set the offset as you explained and see if i sucess!
Thanks again for the reply, really really instructive!

KNOWN tool lengths are from the spindle zero to the tip of the tool. Again, this is fine if you know all of the other dimensions, like the exact location of the top of the part, but do you?

Check with someone there who knows all of this, or I would just start from scratch if you are new to this and the machines operation.

Have fun-----

[miljnor]

For ease of use an repeatability.

Use either: (2) 1-2-3 blocks or (2) 1-2-3 blocks and a tool preset-er to get a 6" distance from table (the center-line for a HRT210) The 6" is unimportant but convenient.

Then get a bad tool holder with no tool in it or a holder that ALWAYS has your tool probe in it, for INITIAL height pick up.

Take both of the above and get a "G" offset set to them (something out of the way, like G150 or something). This will be machine Zero for everything you do from here out.

Now whenever you put a tool in a holder you pick the tool up with that offset and those blocks and you can keep a log of these tools if your so inclined so you can use them in any machine and move them and their offset at will.

For your work, just start with your bad tool holder, or the probe, and pick the Z zero up with that tool ONLY, and you will be able to interchange everything to all your machines and keep track of them.

This might be too much for some but it works well for me and after you get used to it, its second nature.

Still working on a better way to keep track of my tools as they go in and out of the machine.