Question re G76 threading code

More
06 Jun 2016 08:00 #75545 by Clive S
Question re G76 threading code G76 P- Z- I- J- R- K- Q- H- E- L-

I am using a small Myford S7 with single phase motor belt driven (ie no VFD) and a 64 slot encoder disc with 3 opto's A + B + Index on the spindle connected to a mesa 5i25/7i76

Q1. When using an index bit metric 60' set at 90' to the chuck what would be the correct Q value

I have noticed that I have to set K to 2.1 with a Q set to 0 and K set to 1.5 with Q 29.5 to get decent threads

Q2. Using diam mode G7 Is the K value entered as a diam value (ie 10mm thread =1.5)

Q3. Feed & Speed F & S are they relevant in the values when using an encoder

Q4 What is the correct way to make smaller DOC (would that be the R peram)

G0 G40 G18 G80 G21 G49 G95
G90 G7
F300 S450
G0 X10 Z2
G76 P1.5 Z-30 I-.1 J0.1 R 1 K3 Q29.5 L0 E0 H2
g0 X20
g0 Z30
M2

Please Log in or Create an account to join the conversation.

More
09 Jun 2016 10:13 - 09 Jun 2016 10:19 #75713 by cncbasher
Q1
it depends if your using a 60 deg lathe insert ( beware of tip radius here , this needs to be same or smaller than the thread valley) , or a specific threading insert of specific pitch , where most of the work is already done for you ,
if using a threading insert Q = 0 , if a 60 deg standard insert then Q=29.5 .( q is your compound angle )

if using a threading insert then you can cut axiallly at 90 deg , or if usiing a hss single point threading cutter then use the compound
as this reduces the cutting forces as your only cutting on one edge

Q2
K represents the actual thread depth so for metric threads it's easy as your using a 60 deg insert it equals the thread pitch
Q3
feedrate should equal the pitch (unless your doing multistart threads ) , speed = whatever gives you good threads , this depends on the HP available of course , and structural stability .
Q4
the R parameter is the final finishing cut depth
DOC ? do you mean 'diameter of crest ' ?
this is preset when using threading inserts , but using a standard insert , the radius of the insert will give you the
radius of the valley , this coupled with the K value will determine the quality of the crest , and accuracy of dia . so this can be trial and error sometimes . trimming final dia and depth .
cutting too deep with a threading insert will chop the tops off the crest . sometimes making your final dia , just slightly under can help .

when usinig threading inserts the manufacturers data sheet , should have all the information you need

threading can be tricky to find the final sizes the particular machine is capable of .
but once you have a good thread you can usually use the sizes found to relate to other threads quite easily

thread cutting is a novel in it's own right , everyone has their prefered way

a good book on threading and gcode is 'cnc programming handbook by peter smid'
Last edit: 09 Jun 2016 10:19 by cncbasher.

Please Log in or Create an account to join the conversation.

More
19 Jul 2016 11:59 #77635 by Clive S
Sorry for the late reply. Could you just clarifying a couple of points.

Re Q1 If using a standard 60' tip you have said Q = 29.5 .( q is your compound angle ) Does this mean that the tool is set at 90' to the work piece and Linux take care of the compound angle OR is the tool set to 29.5'

Q4. What is the correct way to make smaller DOC (would that be the R peram). What I was trying to ask is that I want to make smaller DOC's ie more passes to cut the thread..

I can now cut decent threads with metric and imperial but would like to cut them with more passes.

Please Log in or Create an account to join the conversation.

More
20 Jul 2016 09:11 #77687 by andypugh

I can now cut decent threads with metric and imperial but would like to cut them with more passes.


The number of passes is controlled by the J and R numbers.

The first cut will be of depth J, the second something like J/R and so on.

linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g76

Please Log in or Create an account to join the conversation.

More
20 Jul 2016 09:28 #77689 by Clive S
Thanks Andy So that will be a bit of trial and error

Any Answer to Q1 as I suspect it may be related?

Please Log in or Create an account to join the conversation.

More
20 Jul 2016 09:50 #77692 by andypugh
The tool should be perpendicular to the work axis, or the thread will be the wrong shape.

Please Log in or Create an account to join the conversation.

More
20 Jul 2016 09:56 #77693 by Clive S

The tool should be perpendicular to the work axis, or the thread will be the wrong shape.

Ok thanks for that.

So using a 60' tool perpendicular Q would be 29.5'

Please Log in or Create an account to join the conversation.

More
20 Jul 2016 11:32 #77697 by andypugh
Q can be anything you want. But some numbers will work better than others.

Lots of debate here: www.practicalmachinist.com/vb/general/se...read-cutting-278289/

Please Log in or Create an account to join the conversation.

More
20 Jul 2016 12:51 #77703 by Clive S

Q can be anything you want. But some numbers will work better than others.

Lots of debate here: www.practicalmachinist.com/vb/general/se...read-cutting-278289/


Yes Andy that is a good read. BUT it is still not clear (to me at any rate) if it refers to manual threading or CNC If you have the tool perpendicular to the job does the Q setting at say 29.5 use that angle with_cnc ie does linuxcnc move the tool in a the Q setting.

Please Log in or Create an account to join the conversation.

More
20 Jul 2016 13:16 #77706 by andypugh
I don't actually understand what you don't understand.

Q is a virtual compound slide angle. The thread forming tool necessarily has to be perpendicular to the work, or it won't form a thread.

Please Log in or Create an account to join the conversation.

Time to create page: 0.082 seconds
Powered by Kunena Forum