Auto tool change

[reece]

Hi Guys,

Having some issues with the auto tool change function, I've got the offsets set up in the auto tool changer and have the input signal set as tool setter input. When I home the machine on initial startup it will home and then move to the correct probe location and run the probing cycle, I have the input set as high on contact and low on no contact. The machine stops as it touches the plate as its supposed to but it is not changing any numbers on the tool offset tab.

I'm then having an issue that during a cutting operation it is not consistently asking for a tool change when required and will not move to the tool change location or do any of the probing cycle.

I'm also having a delay of 50-60 seconds from cycle start to when the machine will start executing the cut profile. It will instantly run the spindle and then just sit inactive for that minute before it starts the cut.

I've attached an example of my gcode. Any help would be appreciated.

Thanks Reece

 

[masso-support]

Hi Reece

Have a look on the F1 screen at spindle settings. Check the spin up time you have set. This will be the cause of the delay before Masso starts machining.

With regards the auto tool changer have you set the tool changer on the F1 screen to manual tool change? Under Manual tool change you set the tool change position and enable the X Y & Z.

In my setup I use the tool change block position to change the tool as it is where it will do the touch off once the change has been made.

Hope this helps

Regards

Peter

 

[reece]

Hi Peter

Thanks for the quick reply, I'll check the spindle delay tomorrow but from memory it's not set to very long at all, as in only 1-2 seconds.

With the tool changer, on the auto tool setter tab I have it enabled and have allocated an x and y position and have both of the check boxes enabled and have set up a z safe distance as well as the tool zero feedrate.

On the Tool changer tab, I've selected manual tool changer and allocated the tool change position as just over the touch plate and enabled all three axis check boxes.

I think everything is set as it should be, the machine homes and touches off on the plate if I home on the f3 screen, but it does not change any tool length settings on the f4 page. If I have tool 2 in at the start of a job that requires tool 1, the masso has not consistently been asking for a tool change even if I hit rewind after jogging to the work offset. It'll only ask after 2 or three attempts of cycle start, followed by feed hold followed by spindle off and rewind again. Once it then asks for a tool change it will not jog over to the touch plate location and go through the proper procedure.

Hopefully everything I've said makes sense, sorry it's a bit of an essay

Thanks Reece

 

[reece]

Hi Guys,

Still having issues with the auto tool change function. I've managed to get the machine to jog automatically once homing to the touch plate and proceed to do the probing cycle, it touches the plate and retracts exactly like in the instructional videos. The issue I'm having is it is not changing the value in the tool offsets tab.

Also if I disable auto tool zero and set a work offset of the end of my cutter on the top of my stock and then move to the f4 screen and auto load the tool offset for tool 1 and then enter G0Z0 in the MDI it as expected stops exactly on the top of the stock. However if I load a new tool for instance tool 2 and once again position the end of the cutter on top of the stock and auto load the tool offset on the f4 screen. If I then enter the MDI command of G0Z0 the bit will plunge through the stock. The masso is not doing the correct calculations for the tool offset.

The only way I can consistently achieve the same cut depth is to change the G54 work offset with each tool change by positioning the end of the cutter on top of the stock and auto loading the G54 Z coordinate to account for the different tool length.

Any help would be awesome, I'm starting to pull my hair out with this thing.

Thanks Reece

 

[breezy]

@reece

I haven't had problems with the Auto Setter, all I did was follow the instructions for Tool Change position and Auto Tool Setter and it worked.

I had G54 set to Zero on all axis. Set the values required on Auto Tool Setter and homed the machine with the longest tool installed. It moved to the Auto touch pad, rapid down to save distance, then at set feedrate until it touched the pad. I then set G54 to the work coordinates and MDI command X0Y0. Then using Z zeroing touchpad set Z zero using G38.2 and G92.

When tool changes were needed the machine moved to the tool change position, changed tool, hit cycle start and the machine went to the tool touchpad and zeroed the tool length and continued machining, with the correct Z settings. When MASSO does the tool length zeroing it adjusts the WCS Z DRO it doesn't change any settings in the F4 screen.

Another important fact is that the gCode must list the Txx tool number before the M06 tool change command.

So to test the operation of the Auto Tool Setter, issue the following string of command in the MDI after you have set Z zero to the top of your stock. You'll need to hit cycle start between tool changes. The tools don't need to be in the tool library on F4 screen.

T01 M06

G1 Z0

T02 M06

G1 Z0

T01 M06

G1 Z0

You should see the Z DRO change when the Auto Tool Setter touchpad is contacted and the tool should just touch your stock.

Regards,

Arie.

 

[reece]

Hi Arie

Thanks for the response, that all kinda makes sense.

The only thing I'm not sure of is your use of G38.2 and G92. My process has been to home the machine, once it has homed, it jogs to the touch plate location and completes the probing cycle with whatever tool was already loaded, T1 for instance. Then I move to my G54 work offset position where the end of my cutter is just above my stock.

I will then command through MDI T2 M6 to call up a tool change to tool 2. The machine will then request a tool change and move over my touch plate and complete the probing cycle. The issue is then that when I move back to my G54 work offset and enter the command G0Z0, the cutter will not stop on the top of my stock. It has not made any change to account for the different tool length, it will either plunge through or stop short.

Is there a step I am missing with the G38.2 and G92 commands. I understand they are a straight probing cycle and a temporary work offset but I am unsure on if and how I have to utilize them.

Thanks Reece

 

[breezy]

Quote from Reece on August 1, 2019, 8:59 am

My process has been to home the machine, once it has homed, it jogs to the touch plate location and completes the probing cycle with whatever tool was already loaded, T1 for instance. Then I move to my G54 work offset position where the end of my cutter is just above my stock.

@reece

At this point you need to zero your Z axis DRO. Then when you do a tool change MASSO should adjust the Z DRO to allow for the new tool length. After the tool change it should return to the same coordinates it was at when the tool change was commanded.

The only thing I'm not sure of is your use of G38.2 and G92.

G38.2 is a probing cycle and G92 is set temp work offset. So I place the touch plate on the job, issue G38.2 F50 which moves the tool down at 50mm/min until it touches the plate then a G92 Z22 which sets the Z DRO at 22mm, (22mm being the thickness of the touch plate). Then I follow it with G0 Z50 to raise the tool clear of the job. All this is in a small gCode file that I auto load with a panel button.

I will then command through MDI T2 M6 to call up a tool change to tool 2. The machine will then request a tool change and move over my touch plate and complete the probing cycle. The issue is then that when I move back to my G54 work offset and enter the command G0Z0, the cutter will not stop on the top of my stock. It has not made any change to account for the different tool length, it will either plunge through or stop short.

Try this test. Set your XY position and Z=0 in G54 on the F4 screen. In MDI issue G0X0Y0Z0 this should move you to the required position with the tool raised, then jog the tool down to touch your job, zero the Z DRO. Jog the tool up to its top position, issue a tool change. The MASSO should move to the tool change position, change the tool, press cycle start. MASSO should move to the Auto Tool Setter and touch the plate, then return to the position it was at when you issued the tool change. Now issue G1 Z0 Fx (Fx being the feedrate you wish the tool to approach the job) and the tool should just touch the job. If the Auto Tool Setter is working correctly the Z DRO zero should have moved in relationship to the machines absolute coordinates.

Regards,

Arie.

 

[reece]

Hi Guys,

Thanks a lot for the help with figuring this out. All sorted now, had the light bulb moment and realized that the issue was from not zeroing off the Z axis DRO on the top of the stock, I had been zeroing off the work offsets with the cutter on the top of the stock and missing that last step in hindsight it's really obvious. As soon as I pressed that button everything worked exactly as it should

Seems like a super simple mistake but it just wasn't very clear that it was a required step from all the videos that I'd watched online.

Once again thanks heaps for the help.