The Craftmans Shop > New from Old
The Sequel - Oh Blimey I bought a CNC Lathe (Beaver TC 20)
awemawson:
--- Quote from: WeldingRod on August 05, 2018, 11:28:01 PM ---Ok, I've gotta ask... my sole reference for chuffed-ness come from the British Baking show. My kids are asking; what is chuffed, and why should someone else need to say.it about you?
I'm might be asking too ;-)
Sent from my SAMSUNG-SM-G891A using Tapatalk
--- End quote ---
"pleased, happy," c.1860, British dialect, from obsolete chuff "swollen with fat" (1520s). A second British dialectal chuff has an opposite meaning, "displeased, gruff" (1832), from chuff "rude fellow," or, as Johnson has it, "a coarse, fat-headed, blunt clown" (mid-15c.), of unknown origin.
awemawson:
Pete the dogs seem fine together :thumbup: Remember we frequently have people with dogs staying in the cottages, in fact the other one has two at the moment, so three extra dogs on site !
Yes switch on moments and trying new operations are definitely stomach clenching moments. Trouble is that this machine has so much power behind all it's movements that it won't take prisoners if you make an error, and metal will be bent!
This morning I've being getting my head round work offsets (G54 etc) as implemented on this machine, and trying to get things set up so things I create in FeatureCAM are all located within the 'safe zone' where spinning chucks and tool turrets DON'T get into intimate contact with each other!
Believe me a 10" chuck spinning at 3500 rpm with 26 kW behind it has an awful lot of stored energy just waiting to leap out and catch you unawares, it also kicks up quite a wind with the jaws acting as fan blades.
The hinge for the Tail Stock access door arrived this morning, but it is really too flimsy for this application. I've ordered a far heavier duty one (2 mm thick) from RS Components that should arrive tomorrow morning. This one has the advantage also that it is un-drilled, so I can pick up and reuse the existing tapped holes in the door frame.
DICKEYBIRD:
--- Quote from: awemawson on August 06, 2018, 06:06:03 AM ---This morning I've being getting my head round work offsets (G54 etc) as implemented on this machine...
--- End quote ---
When you get work offsets working well, could you please take a few extra minutes to describe what you did & how you did it? I read every word in all your threads to trying to learn how to do things right but work offsets coincidentally are especially important to me right now. I've always muddled my way along in Mach3 Turn & never learned how to use work offsets. I just programmed everything in an (what I called) absolute manner. It worked & many parts were made successfully but tool changes were difficult. After finally getting a decent controller & software now, I'm starting over & trying to learn how to do things correctly.
awemawson:
Milton,
When my lathe seeks it's reference points, it finds them at X= 530, Z=660 (millimetres of course) so it then sets up it's co-ordinate system with those positions having those values.
Now on this lathe it uses it's zero reference as the face of the chuck - (the Traub used the chuck mounting face ie the back of the chuck). So if you use a CAD program to produce your G code, which will conventionally use the outermost end of the stock (away from the chuck) as it's Zero Point for Z, then you need some method of 'shifting the zero' . (For a lathe it is really only the Z axis you are worried about until you come to tool length compensation but let's ignore that at the moment)
So this is where G54 'work offset' comes in. There is a screen on the 820T controller under 'settings' that lets me pre-set an X and Z value for the G54 offset command (also for G55,G56 & G57) - I have loaded mine with a Z value of 300 at the moment to keep things well away from the chuck as I am testing.
OK back to the plot - when the controller gets a Z address to move to, it adds it to the Z value stored in the currently active work offset command (Also the tool length compensation value) so if I tell the machine to "G00 Z10.00" it actually moves to Z300 +10 = Z310
By issuing a G53 you can cancel any offsets that are in effect.
Now today I've been using both those commands to ensure that the FeatureCAM post processor that I am tweaking always moves the tool turret to a safe place before a tool change. It has a place that you can pre-set it before running the PP, but then the value it assigns will be massaged by the G54 that is in effect and move to the wrong place.
My solution is to have a little macro always available in the controller thus :
%SPF 54 (Sub Program L54)
G0 G53 G71 G90 G40 D0 X450 Z400 (full speed move to X450,Z400, cancel G54, Metric measurements, Absolute move,cancel cutter radius compensation, no tool offset)
G54 (Reactivate G54 work offset)
M17 (Sub-Program end
Which is called by the main program that the PP generates thus:
%MPF 8
( CUST PART# )
( 8-6-2018 )
N25 G71 G90
N30 L54 P1 (Call Sub Program L54)
N35 T3 D3 ( TOOL 3 EN_TURN_55 )
N40 @714
N45 G92 S3500
N50 G96 S170 M4
N55 M8 (MSG, ROUGH TURN TURN1 )
N60 L54 P1 (Go to safe place)
etc
etc
DICKEYBIRD:
Thanks a lot Andrew, I believe it's finally starting to sink in. When I finish the latest homing sequence update, your tutorial & actually keying it in at the lathe a few times should sort me out! :beer:
Navigation
[0] Message Index
[#] Next page
[*] Previous page
Go to full version