Manual tool change

Post anything you want to discuss with others about the software.

Re: Manual tool change

Postby Battwell » Sun Oct 07, 2018 12:30 pm

if you put in tool length 10mm for tool 1 apply and save in tool table. inset a tool - any tool
now type in mdi g43h1 (tool offset should show as 10mm)
touch off tool and zero g54 offsets x y and z to a known position on your table ( a matchstick of wood clamped out of the end of vice for example - so it cant damage tool)
(this is your work offset. as if you have it set as the corner of a job etc)

now jog tool 1 up away from the matchstick

now tool 2 - set it to 20mm length in tool table ( leave the same tool 1 in the spindle)- make sure you apply the tool length in tool table!
type in mdi. g43h2- enter
press go to zero button. (same as g0 x0y0z0) the tool should now be in the same xy position. but 10mm above (as its 10mm longer)

the m6 doesnt affect tool offset. only g43 makes it change.

from this you will see that after setting your first tool to the job, any tool change after followed by g43h toolnumber will put the correct tool length ready to run.

what you are seeing previously is correct- the z readout is backed off (-Ve) of the new tool length selected. it will only become the same as fixture after a move
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 383
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Manual tool change

Postby gabi68 » Sun Oct 07, 2018 3:29 pm

Battwell wrote:if you put in tool length 10mm for tool 1 apply and save in tool table. inset a tool - any tool
now type in mdi g43h1 (tool offset should show as 10mm)
touch off tool and zero g54 offsets x y and z to a known position on your table ( a matchstick of wood clamped out of the end of vice for example - so it cant damage tool)
(this is your work offset. as if you have it set as the corner of a job etc)

now jog tool 1 up away from the matchstick

now tool 2 - set it to 20mm length in tool table ( leave the same tool 1 in the spindle)- make sure you apply the tool length in tool table!
type in mdi. g43h2- enter
press go to zero button. (same as g0 x0y0z0) the tool should now be in the same xy position. but 10mm above (as its 10mm longer)

the m6 doesnt affect tool offset. only g43 makes it change.

from this you will see that after setting your first tool to the job, any tool change after followed by g43h toolnumber will put the correct tool length ready to run.

what you are seeing previously is correct- the z readout is backed off (-Ve) of the new tool length selected. it will only become the same as fixture after a move



THANK YOU!!! It's working. Now, how can I use the probe (which is the longest tool) with the same procedure?

Thanks again
Gabi
gabi68
 
Posts: 29
Joined: Wed Dec 07, 2016 10:35 pm

Re: Manual tool change

Postby Battwell » Sun Oct 07, 2018 8:12 pm

Exactly the same way
Set your tool probe length as eg tool 96
Touch off and zero your part with that tool
Use that to set your reference point

Every other tool will be the same as setup for tool 2 in above example.

All you need to do then in your code is as follows. Eg tool 2
M6t2 ( put tool 2 in spindle)
Go g43 h2

The z dro will then change and tool length for tool 2 will be loaded from the tool table.

I use a tool length probe to make it all automatic and a lot faster :-)
https://youtu.be/PNkMnU_3v8Y
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 383
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Manual tool change

Postby Battwell » Sun Oct 07, 2018 8:23 pm

Note the g0 added to the g43h2 line
This makes the offset take effect ( without creating a movement)
But the dro will update to correct distance from your work zero position for tool 2
Just play with it until you understand it fully- using safe matchstick method or similar until your brain absorb the info.
Uccnc does exactly what it’s told
Operators don’t lol
Remember GIGO. Garbage in garbage out.
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 383
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Manual tool change

Postby Vmax549 » Sun Oct 07, 2018 9:14 pm

OK I will be teh dummy to ask but what does teh G0 have to do with G43

G0 G43H2 ?? All I see teh G0 do is reset the motion modal value to G0.

The only 2 ways I know that it works is

G43 H2
G0 Z0

or
G43 H2 G0Z0

UCCNC seems to be sensitive to teh correct word order in this case.

Just a thought, (;-) TP
Vmax549
 
Posts: 1380
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: Manual tool change

Postby Battwell » Sun Oct 07, 2018 10:52 pm

I use what I wrote in my macros
It works
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 383
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Manual tool change

Postby gabi68 » Mon Oct 08, 2018 4:27 am

Thank you. I tried the same procedure with the probe and is WORKING. I did not put a G0 before G43Hx and that worked without movement. I was scared to do a G0 and I tried G1 F100 with my finger over reset button. THANK YOU.

Gabi
Did I said THANK YOU?
gabi68
 
Posts: 29
Joined: Wed Dec 07, 2016 10:35 pm

Re: Manual tool change

Postby Battwell » Mon Oct 08, 2018 8:23 am

your welcome. now go make some nice parts
and tell everyone how good uccnc is.
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 383
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Previous

Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 3 guests