[muxster]

tool length compensation usage on dynapath delta 40 there is H registers how to use them in program? when i put the H01 H1 say in line 10 i get 133 format alarm, i want it to use it before line 12 any idea what is wrong. anyone have sample program using tool offsets and manual tool changes.
the program i have runs complete just trouble using tool length compensation.
thanks marc

dynapath
%
N0010(9)T1M04$
N0011E1X0Y0$
N0012(0)Z.1$
N0013(0)X-.3009Y.2083$
N0014(0)Z.025$
N0015(1)Z-.075F35.$
N0016(2)P0D1X-.187Y.1348I-.187J.2598$
N0017(2)D1X-.1825Y.1349I-.187J.2598$
N0018(2)D0X-.175Y.135I-.175J-.075$
N0019(1)X-.075F60.$
N0020(2)D0X.135Y-.075I-.075J-.075$
N0021(1)Y-.95$
N0022(2)D0X-.075Y-1.16I-.075J-.95$
N0023(1)X-.1761$
N0024(2)D0X-.3852Y-.9691I-.1761J-.95$
N0025(2)D1X-.45Y-.91I-.45J-.975$
N0026(1)X-1.8$
N0027(2)D1X-1.8647Y-.9691I-1.8J-.975$
N0028(2)D0X-2.0739Y-1.1601I-2.0739J-.95$

%
N.001O100 (FADAL)
N.002G70G90T10M06
N.003S6000M03
N.004G00X-.3009Y.2083
N.005Z1.H10M08
N.006Z.1
N.007Z.025
N.008G01Z-.075F35.
N.009G17G03X-.1825Y.1349I.1139J.0515
N.010G02X-.175Y.135I.0075J-.2099
N.011G01X-.075F60.
N.012G02X.135Y-.075I0.J-.21
N.013G01Y-.95
N.014G02X-.075Y-1.16I-.21J0.
N.015G01X-.1761
N.016G02X-.3852Y-.9691I0.J.21
N.017G03X-.45Y-.91I-.0648J-.0059

[jagardner4]

How tool length compensation is activated on a DynaPath control depends on the machine tool it's been applied to. View your block N0010 in the Program mode (Mode 3) and see if the H variable is even available. If not, then the tool length activation is probably tied to the T code itself.

It would help to know what kind of machine this control is on and whether you're dealing with a tool changer or not.

[muxster]

this is a knee type chaveler/(brigdgeport style) mill manual tool change no Automatic tool changer. the way they were doing length comp was using the z offset in the E offset page. do you have a example program with the tool comp used

[jagardner4]

Tool length compensation is entered into the T code table. And since this is a manual mill with no tool changer, the T code is used to make the tool compensation active.

The Z axis offset you are referring to is in the fixture offset table and is associated with and activated by E code. I don't think this is what you are looking for.

Your example is fine. The T code (T1) in block N0010 is activating the first tool length compensation in the T table.

[muxster]

if i do not put a Z value in the E1 register the machine over travel (cause .100 clear plane and no tool length applied) although if i put a example -1.0 in the E Z offset register everything ok except i lost 1 inch of quill travel and what to do on the next tool.

do you have example program with tool length and tool changes?

[guru]

On our Dynapath Delta 20

T0101 means call tool#1 and offset#1
T0100 will cancel offset on tool#1

T0210 means call tool#2 and offset#10

[muxster]

thank you guru

i will try that T0101

if i want the machine at the end of the program to return to Z home just have G0T0100 this machine has an air driven motor to unlock the draw bar/release the tool holder i want to put the machine ready for tool change (on the hass/fadal i just put Z0H0 at the end.

and to apply cutter comp use G41D01 is this ok

[muxster]

INSERTING RED TEXT
N0010(9)T101M04$
STILL 133 FORMAT FAULT ALARM

INSERTING RED TEXT
N0010(9)T1H01M04$
STILL 133 FORMAT FAULT ALARM

INSERTING RED TEXT
N0010(9)T1M04$
N0011E1X0Y0$
N0012(0)H01Z.1$
STILL 133 FORMAT FAULT ALARM

[jagardner4]

1. On the control, press the "Mode Select" key, then "3". This will put you into the Program mode.
2. Now press "N", "0" and the "Enter" key. This will enter a sequence number.
3. Now press the "Event Type" key and "9". This will bring up the "M Function" event, where T codes are programmed.
4. Press "T", then "0", then "Enter". Note how many digits show up in the T code field. It will be either 2 or 4 digits. This is the number of digits the control is looking for.
5. Also note if there is an H field. I suspect there isn't. If the field doesn't exist, the control will always give you a 133 format fault when you try to program one. Also, if the H field doesn't exist, the tool length compensation is being activated by the T code.

[muxster]

doing the steps 1 ~5 the control has uses 2 digits for tool not 4 still, confused on apply tool length compensation in part program for the dynapath delta 40

[jagardner4]

Based on your answer, I must assume that the control has a T code table accessible in Mode 6. Each T code in the table will have a Z entry and a D entry. The Z entry is the tool length, the D entry is the tool diameter. Both values are activated when you execute the corresponding T code. The tool length is summed into the Z axis command. Tool diameter won't be used until you call for cutter diameter compensation.

Short version: Your tool length compensation is being called by a 2-digit T code.

[muxster]

i agree with your post but this is what is happening at the control (dynapath) i use hass and fadal vmc's daily and i can use T1 with any H offset example H1 H41

example 1

Z value in the (mode 6 ) H1 register = -1. i cycle start the program below machine over travel (cause .100 clear plane/safety and no tool length Applied/activated machine is ignoring any tool table H data)

example 2

Although if i put a example (mode 6 ) -1.0 in the E Z offset fixture register i cycle start program below everything runs ok but machine moves to -.900 (-1.0 E Z offset + .10 clear plane) and what to do on the next tool T2, T3 ect. as program has other tool changes.

can you copy and try this program in your machine if you get the same as i do in example 1, example 2 the tool tip Z0 is set on the top of the block?

do you need to setup a reference tool master that the other tools link to?


dynapath program example below starting with %

%
N0010(9)T1M04$
N0011E1X0Y0$
N0012(0)Z.1$
N0013(0)X-.3009Y.2083$
N0014(0)Z.025$
N0015(1)Z-.075F35.$
N0016(2)P0D1X-.187Y.1348I-.187J.2598$
N0017(2)D1X-.1825Y.1349I-.187J.2598$
N0018(2)D0X-.175Y.135I-.175J-.075$
N0019(1)X-.075F60.$
N0020(2)D0X.135Y-.075I-.075J-.075$
N0021(1)Y-.95$
N0022(2)D0X-.075Y-1.16I-.075J-.95$
N0023(1)X-.1761$
N0024(2)D0X-.3852Y-.9691I-.1761J-.95$
N0025(2)D1X-.45Y-.91I-.45J-.975$
N0026(1)X-1.8$
N0027(2)D1X-1.8647Y-.9691I-1.8J-.975$
N0028(2)D0X-2.0739Y-1.1601I-2.0739J-.95$

[jagardner4]

Machine Tool Builders such as Chevalier have many parameters available to them on a DynaPath control which specify the way the CNC handles T codes, tool lengths and diameters, as well as fixture offsets. So a Chevalier probably won't act like a Haas or a Fadal (or a Tree, for that matter). It's not right or wrong, it's just different.

I think the reason that activating tool length compensation is causing you to hit a negative limit in Z, which doesn't happen when you activate the fixture offset, is that the tool length compensation is immediate and the fixture offset activation, which is controlled by parameter, has been set to deferred.

There are a couple different ways to handle tool length offsets.

If you set your part zero point (in Z) by touching Z = 0 to the tip of the first tool, then that first tool should have an length offset value of zero. As you touch off the other tools to the same point, the offset entered in the table should reflect the length difference of each tool from that first tool.

If your part zero (again, in Z) is referenced from the face of the quill, then every tool, including your first, will have a non-zero offset representing the distance from the tool tip to face of the quill.

Not knowing the way in which Chevalier chose to set up the Z axis or how you are setting your part zero in Z, I can only guess at the cause of your issue, but I would have thought the tool length offset in your case would be a positive number. Once the tool length offset is pulled in, the position of the Z axis should be the part zero position + tool length offset. In other words, Z would need to go positive some distance to accomodate the length of the tool.