[leeko]

Hi all,

I'm having a hard time wrapping my head around setting my Z offsets for parts and tool lengths in the dynapath control.

If I'm reading the manual correctly, it suggests touching each tool off on the top of the part (or wherever the WCS origin will be), and then setting reference zero for the part in the jog screen using a longer reference tool whose length never changes.

I think I see how this works, but it's different than the workflow I use on my haas at work. There, I touch each tool off on a 4" block set on the table, then use one tool to touch off on the part and calculate the difference in z height for that one tool. I then enter the difference between that tool's length and the part touch-off length as my z value for G54. I don't see how to replicate this workflow on the dynapath - can anyone advise? Or is there a better way of doing this?

Thanks in advance,

Lee

[cngbrick]

Leeko,

There is no G54 in Dynapath, it uses the work offsets table (E).

The way I set tool length offsets:
1) Tool setter (or 123 block with feeler gauge) on table
2) Reference tool in spindle (I use a 1 inch gauge pin permanently mounted in a tool holder, about as long as my longest cutting tool)
3) Bring down ref tool on tool setter, press 9 and toggle Z axis jog switch to set temporary Z zero
4) Swap tool and bring down on tool setter, select tool number in table and set tool length, repeat for all tools
5) When done reset Z reference.

I then use the reference tool to set my work coordinates (E) for jobs. In practice, 75% of my work uses the bottom left hand corner of my main vice jaw (E1), 10% is off my 4th axis chuck (E4) and the rest I set with the reference tool.

Since the reference tool is used to set work coordinates all tools will automatically have their offset from the work coordinates as well.

Does that answer your question?

RT

[leeko]

Hi RT,

I think so - what was tripping me up was that (I think) the control doesn't seem to show the absolute position of the tool as you're jogging - only the relative position to the reference zero. So, I couldn't figure out how to set the difference between the tool length on the tool setter and the tool length on the workpiece. If I understand your steps correctly, you use the temporary z zero on the tool setter then reset it to the workpiece Z0 (G54 equivalent or E01 in dynapath terms) - that way the control does the math, and you don't have to calculate anything for the Z height value.

Does that sound right?

Thanks again!

Leeko,

There is no G54 in Dynapath, it uses the work offsets table (E).

The way I set tool length offsets:
1) Tool setter (or 123 block with feeler gauge) on table
2) Reference tool in spindle (I use a 1 inch gauge pin permanently mounted in a tool holder, about as long as my longest cutting tool)
3) Bring down ref tool on tool setter, press 9 and toggle Z axis jog switch to set temporary Z zero
4) Swap tool and bring down on tool setter, select tool number in table and set tool length, repeat for all tools
5) When done reset Z reference.

I then use the reference tool to set my work coordinates (E) for jobs. In practice, 75% of my work uses the bottom left hand corner of my main vice jaw (E1), 10% is off my 4th axis chuck (E4) and the rest I set with the reference tool.

Since the reference tool is used to set work coordinates all tools will automatically have their offset from the work coordinates as well.

Does that answer your question?

RT

[cngbrick]

leeko,

That's it in a nutshell. That temporary zero set is the key to the whole thing.

Once you set your tool lengths this way then you can use the ref tool to set your work offsets and the end of the ref tool is Z zero wherever you decide to place it, whether stock top, fixture top, table top, etc. I keep four static work offsets on my system: fixed jaw location for two Kurt vises, 4th axis chuck and in E32 I keep the coordinates of a safe tool return location that my post processor uses to position tools when I need to reposition the 4th axis.

RT

[leeko]

Thanks CNG

I just finished trying that sequence, and it makes sense to me.

Unfortunately, as soon as I started drip feeding my machine rapided to X- and Y- extents until the Y limit switch tripped. Not sure exactly what happened, but I'm guessing it's because I left the wcs in fusion360 as "0" - this defaults to G54 for haas machines, I figured it would default to the machine zero coordinates I set in jog mode. Apparently not? I'll try specifying E01 as the fixture offset / WCS next. I assume if I've set the machine zero as the touch off point on the part, I can leave E01 in the fixture offsets table as 0,0,0?

Thanks again

Lee

leeko,

That's it in a nutshell. That temporary zero set is the key to the whole thing.

Once you set your tool lengths this way then you can use the ref tool to set your work offsets and the end of the ref tool is Z zero wherever you decide to place it, whether stock top, fixture top, table top, etc. I keep four static work offsets on my system: fixed jaw location for two Kurt vises, 4th axis chuck and in E32 I keep the coordinates of a safe tool return location that my post processor uses to position tools when I need to reposition the 4th axis.

RT

[cngbrick]

Yes, always pick a non-zero coordinate system in Fusion 360. Normally the post-processor should flag this I believe.

Also, make sure you have set the work coordinates you will use and that you re-homed Z if you set a temporary Z for your tool offsets.

RT

[cngbrick]

Sorry, missed the last part of your question.

Work offset: bring your ref tool to your desired coordinates to set the work coordinates, go into the E table and set zero for each coordinate in turn. This will register a distance from your machine homing switch locations, not 0,0,0.

RT

[leeko]

Sorry, missed the last part of your question.

Work offset: bring your ref tool to your desired coordinates to set the work coordinates, go into the E table and set zero for each coordinate in turn. This will register a distance from your machine homing switch locations, not 0,0,0.

RT

Will do, thanks

I did do that last time around, but it was for "part program zero set" on the jog screen rather than the fixture offset.

If I'm setting the part touch off point in the fixture offset, does that mean I don't need to do that in "part program zero set"? What's the purpose of that setting, if not for setting the wcs touch off?

Sorry for all the questions!

Lee

[cngbrick]

I'd have to have a look at my manual when I'm back in the office, but I believe the intent is to "facilitate" programming right off the machine. It's not much of a time saver as you have to rezero everytime you powerup the machine.

For normal operation, the machine should be homed on the switches at startup and then work coordinates referenced from there. Don't set any other zeros outside of the work coordinates menu (E).

RT

[leeko]

I'd have to have a look at my manual when I'm back in the office, but I believe the intent is to "facilitate" programming right off the machine. It's not much of a time saver as you have to rezero everytime you powerup the machine.

For normal operation, the machine should be homed on the switches at startup and then work coordinates referenced from there. Don't set any other zeros outside of the work coordinates menu (E).

RT

Ah, I didn't consider the conversational side

Thanks!

[leeko]

Probably dumb question: how do I reset the "9 - zero set" Z height, after temporarily setting it for the tool height setting? I don't see an option to reset

Lee

[cngbrick]

Once your are done? Ref zero (R + Z jog switch) on Z axis as you would on startup, no need to redo the other axes this time.

RT

[leeko]

Once your are done? Ref zero (R + Z jog switch) on Z axis as you would on startup, no need to redo the other axes this time.

RT

Thanks!

[leeko]

Thanks!

Got it all working, thanks to your instructions - thanks again!

Then I quickly burned up a 1/2" drill running too fast in 4140. Oh well - at least that's a problem I'm more familiar with how to fix

Next question, though - is entering the fixture offsets really a matter of writing them down from the jog screen, then entering them manually on the fixture offset screen? That seems quite an error prone way of doing...

Lee

[machinehop5]

Next question, though - is entering the fixture offsets really a matter of writing them down from the jog screen, then entering them manually on the fixture offset screen? That seems quite an error prone way of doing...

Lee

Hi Lee...after Jogging to fixture location..go into Mode Select >(6)Tool Tables>then pick the Offset number you want....then there should be a Fixture Calibrate soft key at bottom of screen......or maybe D20's did not have that option? If, it does Hit x or y or z then softkey it to enter current position. Works the same for Tool comp hopefullly

DJ

[leeko]

Hi Lee...after Jogging to fixture location..go into Mode Select >(6)Tool Tables>then pick the Offset number you want....then there should be a Fixture Calibrate soft key at bottom of screen......or maybe D20's did not have that option? If, it does Hit x or y or z then softkey it to enter current position. Works the same for Tool comp hopefullly


DJ

Hi DJ,

I didn't see a fixture calibrate soft key - maybe you're right that the D20 doesn't have it. Dang, that's a pain...

Can anyone else with a Delta 20 confirm?

Thanks

[leeko]

Just checking back to this, something occurred to me:

Does this process for setting tool lengths work even if the height of the knee changes? I *think* it does, because the tool lengths are being set relative to the reference tool (which is calibrated to zero) each time.

So, if I change the height of the knee (and therefore the toolsetter), I can still add new tools as long as I've set that temporary Z zero beforehand

Do I have that right?

Thanks,

Lee

[cngbrick]

As long as you use the same ref tool with the temporary zero it works at any surface that you touch off.

RT

[leeko]

As long as you use the same ref tool with the temporary zero it works at any surface that you touch off.

RT

Awesome, thanks

I was worried I'd have to re-touch off all my tools every time I move the knee

Lee

[machinehop5]

yo leeko... The fast way and most likely easiest with your KM type machine Z0 is machine Home all the way Up....the distance between Home and Gage Block size (of programmers choice) is the number input into the Offset number for each Tool...the value will always be a minus value(-xx.xxxx)

Good hunting,
DJ