Content Preview
TB170 Rev 3 Γ’ Thread Repair Thread Recut on a Centroid CNC control
Overview
This document describes how to pick up and recut an existing thread on the Centroid lathe CNC
control The example here assumes external threads that are cut from right to left However the same
techniques can be used on internal threads and left to right threads as well
Thread recut procedure in steps
1 Load the part
2 Index the spindle
3 Program the thread in Intercon
4 Touch off on a good section of the existing thread
5 Teach in and then reset the Γ’Thread FaceΓ’ position in the Intercon thread program
Thread recut procedure in words The operator simply has to rotate the spindle to an index location
and then jog the tool to align it with an existing thread At that point the operator cursors to the
Γ’Thread FaceΓ’ coordinate in the threading canned cycle and then press the Teach Γ’ZΓ’ key to teach in
the touch off position Then simply add a distance divisable by the thread lead to that value so the
thread starts at the beginning of the threaded part or just beyond it
Follow these steps
1 Load the part Load the damaged threaded part into the chuck and dial it in so that the threaded
workpiece is concentric with the spindle and runs true
2 Index the Spindle Identify and mark the spindle Index location This is accomplished by having the
control show us where the spindle index pulse is located as the operator slowly rotates the spindle by hand
Once the index location is identified mark the spindle location so it is easy to reposition the spindle back to the
index location Note Once the spindle index position has been identified and permanently marked on the
machine the steps below describing how to identify the index will not have to be repeated for any future thread
repair
a Depress Estop Go to the PID screen Press Γ’F1Γ’ Setup Γ’F3Γ’ Config type in password 137 press enter Γ’F4Γ’
PID
b Now slowly r otate the spindle by hand put the gear box in neutral and once every revolution of the spindle
the index position will appear beside the spindle axis label usually the 5 th
or 6 th
axis label and spindle axis label
is typically labeled Γ’NΓ’ The spindle index location is identified by an asterisk this asterisk will appear beside the
axis label like so N*
Now s lowly turn the chuck by hand until the asterisk Γ’*Γ’ appears on the screen If you passed by it turn back and
forth slowly until the Γ’*Γ’ stays on the screen beside the spindle axis label
c Now mark this spindle location in some clear and impervious manner And press ESC several times to return
to the main menu
3 Program the Thread using Intercon Threading Canned Cycle
a In Intercon Select Γ’F5 Thread Γ’ and e nter all the thread information as usual except the Γ’Thread FaceΓ’ and
Γ’ClearanceΓ’ value
Press Γ’F7Γ’ Details and complete the thread data entry
b After you've entered the thread data figure out what the First Cut pass Diameter will be for the programmed
First Cut Depth in the threading cycle We will use this First Cut Diameter to line the tool up with the existing
thread!
The first pass diameter of the threading cycle will be made at the Major Diameter minus 2x the First Cut Depth
The First Cut Depth is determined by the operator In our case we chose 01Γ’ for a First Cut Depth
For our 1 7/8 16 external thread the Major Diameter = 1 8703Γ’ and we decided to program the First Cut Depth
at 010Γ’ so Intercon will make the first cut at this diameter 1 8703 Γ’ 2* 01Γ’ = 1 8503Γ’ as the First Cut Diameter
for this threading cycle Make a note of this First Cut Diameter as its used in Step 4 below
4 Touch off the Threading tool to a Location of the Existing Thread that is not Damaged
a Set Z and X offsets for the threading tool and any other tools you will be using as usual
b Set the Z axis part zero at the end of the part or at your customary location
c If the offsets for the threading tool are not already active as displayed in the status box in the upper right
corner of the screen then activate them using the MDI prompt For example to activate tool offsets for tool
press F3 for MDI and enter the command T0505 then press CYCLE START Press ESC to leave the MDI
prompt
d Turn the spindle around to the index pulse position using the spindle index mark that you located earlier in
Step 2
e Touch off the tool on the left flank of the first full good thread
Position the threading tool in the middle in Z of a good thread carefully jogging the tool tip between the crests
of the first two fully formed threads now jog X to the first cut first pass that the threading cycle will make as
programmed in Intercon diameter Slowly and incrementally jog the tool tip right Z+ until it just touches the left
flank of the first full good thread Note the Z axis position on the DRO
5 Set Γ’Starting ZΓ’ Position in the Intercon Program using Teach
a In Intercon Press Γ’F9Γ’ Teach Mode to display the Teach Mode DRO on the Thread Cycle Screen
b Highlight the "Thread Face" value in the threading operation
c Teach in the Z touch off position Press "Z" on the keyboard to copy the Z position from the Teach DRO
to the Thread Face field in Intercon
You now have a thread start position that is synchronized with the existing thread The only problem is that
it is already on the thread and you probably don't want to start threading at the touch off position you want
to start at the beginning of the thread or better yet further out in air before the thread starts So let's start
some whole number of thread turns out to the right Typically you would add enough thread distances that
the threading cycle will start to thread in air beyond the beginning of the part The proper starting Z position
is also dependant on the Thread Infeed Angle There are two cases when figuring out a proper starting Z
position one where the Thread Infeed Angle is = 0 equal front back loading on the threading tool and one
where the thread infeed angle is not 0 common value is 59 degrees Thread Angle Γ’ 1 degree Don't
know which one to use? The simpilest is using a Thread Infeed Angle of 0 equal tool loading front to back
Thread Infeed Angle of zero simple runs the tool down the middle of the threads for thread recutting this
typically is fine since the tool usually isn't doing a lot of work just cleaning up a damaged area
d To calculate a Starting Z value with a Thread Infeed Angle of 0 press Enter to modify the Thread
Face value and add several times the thread lead to the value you got from the Teach DRO In our example
we need about 1/2Γ’ from the touch off position to start the thread clear of the part 1/2Γ’ is an even multiple
of our thread lead exactly 8 threads So adding 5Γ’ to the touch off position of 1902 yields a Thread Face
value of 3098Γ’
For more complicated thread pitch calculations you can use Intercon's expression calculator With the
cursor on the Thread Face Z value press enter and then type "=" and now cursor to the right of the touch
off value 1902 using the Γ’ >Γ’ right arrow key and add a distance to the Thread Face Value that is an even
multiple of the thread pitch In our example the pitch is 16 thread per inch with yields a distance of 0625Γ’
per thread 1Γ’/16= 0625Γ’ So we just eyeball the number of thread distances to add in our case its about
8 threads to be beyond the actual start of the threads So we will add 8 times 0625Γ’ to the Taught in
Thread Face Z value 1902 touch off position + 8 threads* 0625 thread lead = 3098Γ’ is our real Thread
Face Z value
e To calculate a Starting Z value with a Thread Infeed Angle of 59 degrees Perform the calculation
in the step above and add the value that results from this calculation TAN Thread Infeed Angle/2 *First
Cut Depth In our case TAN 59 ΓΒ° /2 X 01Γ’= 00566Γ’ So add 00566Γ’ to 3098Γ’ calculated in part d above
for a new starting Z value of 3098Γ’ + 00566Γ’= 0 31546Γ’
f Now set the Ending Z value to some reasonable position at the end of the thread If the thread ends in a
relief groove then you can stop the cut anywhere in the groove If the thread ends in a chamfer out then
you should error on the side of chamfering out early In any case Ending Z does not need to be
synchronized the way Starting Z does
6 Post the Intercon program and run the program to recut the threads just like any other job
Notes
1 Special Conditions Sometimes it is not always easy to touch the tool off a thread at the First Cut pass
Depth You may need to jog the tool deeper into the thread a smaller diameter in order to reliably touch off a
good thread flank In this case to determine the Thread Face value in Intercon you will have to adjust the
resulting deeper touch off Thread Face value by following the T hread Infeed A ngle back out to the Major
diameter
To calculate the proper Starting Z while deeper in the thread use this formula
Major Diameter/2 Γ’ Tool Touch Off Diameter/2 *TAN 1/2 Thread Infeed angle = Amount to add to Starting Z
value
MD /2 TTOD /2 * TAN ΓΒ½ Thread Infeed A ngle = Amount to add to Starting Z in Intercon
For example we are using a Thread Infeed Angle of 59 Degrees and we programmed the First Cut to be at a
diameter of 3 860" with a Major Diameter of 3 880Γ’ but we have to go in to a 3 790" diameter to locate the
thread Calculate the Amount to add to the Thread Face Z value in Intercon
3 8 8 0Γ’/2 Γ’ 3 790Γ’/2 * TAN ΓΒ½ of 59 degrees =
1 9 4 Γ’ 1 895 * TAN 29 5 =
045 * 56577 = 02546Γ’
Now add 0 02546" to the Thread Face Z position that you got off the Teach DRO
This is the Thread Face Z value
If you don't have a calculator handy you can do this calculation with InterconΓ’s built in expression calculator
Right after you touch off and teach in the Γ’Starting Z ValueΓ’
While the cursor is on the Starting Z value Press Enter to modify it and then type Γ’=Γ’ and Press Γ’ >Γ’ right
arrow key to move the cursor to the right of the value now type after the Z value Γ’+ Tan 29 5 * 090/2 and press
enter 090Γ’ in this example is the MD TTOD
Now to start the threading cycle before the actual threads add some thread distance to start the thread recut
cycle before the actual threads Follow the same procedure as in Step #5 above
2 Clearance Amount In our example we did not use the Clearance amount feature in Intercon since we
programmed our Z face value out away from the actual Z face so the thread would start in air out beyond the
threads If you need to add more clearance room so that the threading cycle starts further away from the actual
thread usually to give the spindle time to get up to speed Simply enter a distance that is a multiple of the
Thread Lead for the Clearance value Our example Lead was 16 threads per inch so any distance amount that
is divisible by 0625 1/16 would be a proper clearance amount Clearance amount is Incremental from the
Starting Z face value
3 Γ’Thread AngleΓ’ Intercon is referring to the Cutting Compound Angle also called Thread Infeed Angle For
example a common 60 degree thread the Γ’Thread AngleΓ’ value in Intercon is commonly set to 59 degrees a
degree less than the thread angle This loads the front of the cutter more than the back A 0 value for Γ’Thread
AngleΓ’ produces even loading of the threading tool front and back of insert is loaded the same and cuts in the
middle of the threads Setting the Γ’Thread angleΓ’ to 59 loads the cutting insert to one side this is called a
Compound Infeed Angle and makes for a better smoother cut
Intercon and G76 can do both types and all "infeed" angles in between
4 Intercon will use the Γ’First Cut DepthΓ’ and the Γ’Minimum Cut depthΓ’ determined by the operator
material and tooling dependent to make automatic multiple passes from the Major Diameter to the Minor
Diameter
5 Find Marker Pulse on some older CNC controls with AC servo motors In the PID screen press Γ’F8Γ’
Drive to get the marker pulse to show