Proper tool setting, Cent 6 and 7

[garnetram]

Does anyone have any good info for setting tool hieghts and part zero on Milltonics VM machining centers?

I have a manual but it does not cover this area.

Thanks

[Dave1]

99.9 percent of the time my Z zero is the top of the part. I use the auto (kinda) tool set procedure. Hit the run key and then F9 I believe is the tool set button. A automatic program will start, It'll ask for height of preset (I use a post it note it's about .003) then it'll load the tool you tell it to, touch off the tool and hit enter, it'll ask for a diameter or radius (depending how the parameters are set) hit enter to set. Then it asks for another tool number or you can finish by escaping out of the screen.
HTH's

Dave

[jpawelk]

Tool setting can be completed in different ways. Your machine may have the tool set program installed and if so that is the easiest way to set the height offset and diameter for all your tools. It can be accessed by pressing F4(run) from the main menu, then HELP(TlSet). This will run a program that will prompt the operator to set the tools. Tool setting can be done is jog and/or hdw. Once in those menus, move the Z axis to your desired location and then press the F key labeled Z Tool. If you have further questions feel free to call Milltronics service at 952.442.1401.

[single phase]

Also, notice what the "Z" value of each of the user coordinates is set at. This will matter if you go to switch to another coordinate (ie G55) because all the tools will follow.

[msomerville]

I usually use the jog or handwheel method. I haven't used the tool set function I will have to give that a try although it seems pretty easy now.

[chipsinpan]

I have never heard of a tool set function , but then I am running Cent 5.
I just run the tool down with HDW , hit tool /tool # /enter/ tool dia (ignore if cutter comp is not reqd) /enter . visual check to see if Z zeros out on the display . If z does not zero out , then the tool in the spindle is not the one you are setting . Check which tool the carousel is at .

[Dave1]

Both my mill's have Cent 5 controls. Cent 5.169 revision and it's there in the run menu, look for the tool set button, it's towards the far right. Once you start using it you'll probably not go back to the way you were doing it.
Dave

Originally Posted by chipsinpan I have never heard of a tool set function , but then I am running Cent 5. I just run the tool down with HDW , hit tool /tool # /enter/ tool dia (ignore if cutter comp is not reqd) /enter . visual check to see if Z zeros out on the display . If z does not zero out , then the tool in the spindle is not the one you are setting . Check which tool the carousel is at .

[single phase]

Another thing about the workstation offsets, if you touch off several tools at the start of a job you can use this procedure to make it easy and accurate to touch off other tools after the start of the job. This makes it easy to retouch another tool later without needing to touch your part (sometimes the surface on the part has been cut away or it has a burr on it). Also this makes it easy to later change the height of your stock or change to another workstation that has a different zero height.

1) Zero all your workstation "Z" values.

2) Touch off and record height offsets of all your tools on the same place on top of your vice with a gage block or off of the table with a gage block. Dave1 is right about using the tool set function built into the control, it is nice because it accounts for the gage block.

3) Use just one of the previously completed tools from step 2 to now touch off the part with a gage block. Jog over in X or Y and then jog down the amount of the gage block. Now your tool should be positioned directly at the desired height of the part. Go to parms/coords/G5X and edit the Z component to be exactly what the Z position of the display reads. This will move "all" the tool heights to the zero of the part.

4) If later you need to touch off a resharpened tool just temporally switch to a workstation that has a zero Z value and use the same above procedure to touch off the tool. Don't forget to switch back to your original workstation.


Cheers
SF

[panaceabea]

on the cent7 when in handwheel mode the f6 button sets tool off set. I touch off on a 1" thick block on the table , hit f6 enter offset 1" , enter then tool diam enter and its set . Its not highligted but f8 is handy, when you touch off on the top of the workpiece with a tool then hit f8 it sets the workpiece z axis zero