Conquest 42 threading cycles

F

FaustoShuguli

Plastic

Joined

Dec 18, 2018

• Dec 18, 2018

• #1

Hello everyone

I have a Hardinge Conquest 42 that is set to work in inches/minute, and the threading cycles are not working (G32, G76)
I have tried G32 Z-0.15 F0.0313 for 10-32 thread but the machine does not move

I have also tried S960 M3 and G32 G98 Z-0.15 F30 but it will not move

What command do I need to have the threading cycles work?

Thank you

 

F

FredC

Diamond

Joined

Oct 29, 2010

Location

Dewees Texas

• Dec 18, 2018

• #2

I have a GT with the 18T control and on it the G76 threading cycle need to separate G76 lines on with parameters for the thread and another with the usual info. I do not single point that often and have to spend some time studying each time I do an new single point thread.
Looked at your post again threading in inches per minute with a G98 in the line? Is that even possible? Why not inches per rev. No spindle encoder?

 

F

FaustoShuguli

Plastic

Joined

Dec 18, 2018

• Dec 18, 2018

• #3

FredC said:

I have a GT with the 18T control and on it the G76 threading cycle need to separate G76 lines on with parameters for the thread and another with the usual info. I do not single point that often and have to spend some time studying each time I do an new single point thread.
Looked at your post again threading in inches per minute with a G98 in the line? Is that even possible? Why not inches per rev. No spindle encoder?

Click to expand...

Coul you pleasr provide a sample of theading cycle for a 10-32
Thanks

 

F

FredC

Diamond

Joined

Oct 29, 2010

Location

Dewees Texas

• Dec 18, 2018

• #4

The only 10/32 or 5mm thread we have done on the GT was behind a shoulder with an thread mill.
Here is a sample of what our machine looks for:
(7/16 FINE THREAD))
T26X.49834Z.25
G76P010000Q00100R.0
G76X.3749Z-.695P03067Q00970F.05
G01
The manual has a bunch of formulas for doing the Parameter line. We do so few that I have to spend some time working it out. I do not think this will help the OP, though.

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Dec 18, 2018

• #5

If 2-line:

G76 P010160 Q00100 R00100
G76 X.147 Z-.15 P01970 Q00980 F.0312


0 = If it is an "SP" model machine

All depends on what year and what control that you have.
I kan't hep with 1-line programming.


--------------------

Think Snow Eh!
Ox

 

F

FaustoShuguli

Plastic

Joined

Dec 18, 2018

• Dec 19, 2018

• #6

Hello
I just tried the codes then the machine moved the entry in X but then it stops in Z
The machine doesn't move in Z with G32 or G76

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Dec 19, 2018

• #7

Ox said:

All depends on what year and what control that you have.
I kan't hep with 1-line programming.

Click to expand...

So again - what year and what control?

0T or 18T are the likely choices - depending on the year.

Maybe your machine takes a "1 line" threading code?
Someone else would hafta hep you with that.


--------------------------

Think Snow Eh!
Ox

 

F

FaustoShuguli

Plastic

Joined

Dec 18, 2018

• Dec 19, 2018

• #8

Tha nachine has control O-T,
Year: 2002

 

T

Tom

Cast Iron

Joined

Mar 18, 2003

Location

Upstate New York USA

• Dec 19, 2018

• #9

will the machine feed in either IPR with the spindle running? Try the following in either MDI or AUTO modes this will determine if you have a spindle encoder feedback problem or not. I am guessing the spindle encoder is faulty as the G32 line you from your first post should have moved the Z axis
M3S500G97
G1G99W-.2F.01

Tom

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Dec 19, 2018

• #10

It heps when you give us all the pertinent info.

So then it is a Conquest T-42 with an 0i-T control maybe?

If so - it should take the 2-line program.

Does the Z axis work otherwise?

Will it feed in G99?

I'm guessin' that you somehow lost your spindle encoder.
I don't know if that's the same as the one used for G99 or not?



edit:

That putz Tom snuck in ahead of me....


---------------------

Think Snow Eh!
Ox

 

F

FaustoShuguli

Plastic

Joined

Dec 18, 2018

• Dec 19, 2018

• #11

Tom said:

will the machine feed in either IPR with the spindle running? Try the following in either MDI or AUTO modes this will determine if you have a spindle encoder feedback problem or not. I am guessing the spindle encoder is faulty as the G32 line you from your first post should have moved the Z axis
M3S500G97
G1G99W-.2F.01

Tom

Click to expand...

Hi,
I have tried G1G99W-.2F.01, the machine does not move.
Is this a spindle encoder problem??

 

F

FaustoShuguli

Plastic

Joined

Dec 18, 2018

• Dec 19, 2018

• #12

Hi,
The machine is a conquest 42 with one spindle, control O-T, (one line programming)
the machine has been configured in inch/min (ACT.F)

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Dec 19, 2018

• #13

Then it's not a 2002.
I don't even think that they were still building "T"-42's in 2002, but maybe...


----------------------

Think Snow Eh!
Ox

 

F

FaustoShuguli

Plastic

Joined

Dec 18, 2018

• Dec 19, 2018

• #14

You right,
There is a mistake in the machine year, the machine is 1990
FS2000

 

T

Tom

Cast Iron

Joined

Mar 18, 2003

Location

Upstate New York USA

• Dec 20, 2018

• #15

If the machine will not feed in G1G99 mode then you have a spindle encoder issue, could be the encoder, the wiring or possibly a belt - I believe that there is a timing belt from the spindle to the encoder on those. The same spindle encoder system is used for both IPR (G99) and all threading commands G32, G92, G76.
On a side note unless someone changed the machine to the Fanuc System Type 10/11 then the G76 threading cycle is a 2 line callout (this was the standard setting on machines shipped), the type 10/11 format is a single line call out and was an option at the time

Tom