Orac MWP84 to use “DO-LOOP” & “SCREW-CUT EXTERNAL THREAD"

All info relating to the Denford ORAC CNC lathes

Moderators: Martin, bradders, Steve, Mr Magoo

Post Reply
Ridgeback
Posts: 33
Joined: Sat 31 Oct , 2015 21:33 pm
Hardware/Software: Denford Triac with original hardware/software
Denford Orac recently updated with Mac3
Location: Redhill, Surrey. U.K.

Orac MWP84 to use “DO-LOOP” & “SCREW-CUT EXTERNAL THREAD"

Post by Ridgeback » Sun 05 Mar , 2017 20:47 pm

Orac MWP84 Initial Setup Guide to: use a “DO-LOOP” & “SCREW CUT” an external thread .
(Issue. 1. Mar 2017)

Turn machine “ON” at mains switch (13 Amp socket outlet).
Wait a minute or so for the m/c to warm up & show info on the Green Screen display.
Chuck should have no resistance if turned manually.
You should have a basic program ready to enter into the m/c to begin with. (Use the example below.)
I will be using an aluminium bar 25.4mm diameter x 65.0mm long.

Green Screen display, press (5) ENTER NEW PROGRAM.
On the “DATA INPUT” pad, press 5, press E (this will take you to page 1 to begin your program).
Press the Double Down Arrows (DDA) to continue to the next page, when finish entering data.
Pg1. “DATA INPUT” Press G70/G71 (G70 = Imperial measure, G71 = Metric measure). DDA.
Pg2. “DATA INPUT” Press G90/G91 (G90 = Absolute measure, G91 = Incremental measure). DDA.
Pg3. “DATA INPUT” Press G50 (G50 = X & Z Datum positions). Enter X 25.0 E, Z 5.0 E. DDA.
Pg4. “DATA INPUT” Press M03 (M03 = Spindle ON in CW direction). DDA.
Pg5. “DATA INPUT” Press G00/G01. (G01 = controlled feed rate, G00 = rapid feed rate, 1200 mm/min max). (This is to move the tool to near the start of the cut.) “X” 13.0 E, “Z” 0.0 E, FEED RATE 500 E, TOOL – No 1 E, SPINDLE – SPEED 1200 E, DDA.
Pg6. “DATA INPUT” Press G00/G01. “X” 0.0 E, “Z” 0.0 E, FEED RATE 100 E, DDA.
Pg7. “DATA INPUT” Press G00/G01. “X” 12.5 E, “Z” 0.5 E, FEED RATE 1000 , DDA.

(Start of Do-Loop).

Pg8. “DATA INPUT” Press G73. “COUNT” 13 E
(Number of passes needed. 12.5mm (start rad) - 6.0mm (finish rad) =6.5mm (amount to be removed) divided by 0.5mm (per pass, as shown on Pg 10 “X”-0.5) = 13 passes).
Pg9. “DATA INPUT” Press G91. (Change to Incremental).
Pg10. “DATA INPUT” Press G00/G01. “X” -0.5 E, “Z” 0. E, FEED RATE 100 , DDA.
Pg11. “DATA INPUT” Press G00/G01. “X” 0. E, “Z” -30.5 E, FEED RATE 100 E, DDA.
Pg12. “DATA INPUT” Press G00/G01. “X” 0.25 E, “Z” 0. E, FEED RATE 1000 E, DDA.
Pg13. “DATA INPUT” Press G00/G01. “X” 0. E, “Z” 30.5 E, FEED RATE 1000 E, DDA.
Pg14. “DATA INPUT” Press G00/G01. “X” -0.25 E, “Z” 0. E, FEED RATE 1000 E, DDA.
Pg15. “DATA INPUT” Press G06

(End of Do-Loop)

Pg16. “DATA INPUT” Press G91/G90. (Change back to Absolute).
Pg17. “DATA INPUT” Press G00/G01. “X” 7.0 E, “Z” 0.0 E, FEED RATE 1000 E, DDA.
Pg18. “DATA INPUT” Press G00/G01. “X” 0.0 E, “Z” 0.0 E, FEED RATE 100 E, DDA.
Pg19. “DATA INPUT” Press G02/G03. “X” 6.0 E, “Z” -1.0 E, FEED RATE 100 CW R20.0 , DDA.
When selecting the G02/G03 block, the way to choose either CW or CCW,
is carried out by moving the cursor to just below the direction you DO NOT want and delete it by pressing the “D” key at the bottom R.H. side on the “DATA INPUT” pad.
Pg20. “DATA INPUT” Press G00/G01. “X” 6.0 E, “Z” -12.0 E, FEED RATE 100 E, DDA.
Pg21. “DATA INPUT” Press G00/G01. “X” 5.1 E, “Z” -12.5 E, FEED RATE 30 E, DDA.
Pg22. “DATA INPUT” Press G00/G01. “X” 5.1 E, “Z” -15.0 E, FEED RATE 50 E, DDA.
Pg23. “DATA INPUT” Press G00/G01. “X” 6.0 E, “Z” -15.0 E, FEED RATE 100 E, DDA.
Pg24. “DATA INPUT” Press G00/G01. “X” 6.0 E, “Z” -30.0 E, FEED RATE 100 E, DDA.
Pg25. “DATA INPUT” Press G00/G01. “X” 11.5 E, “Z” -30.0 E, FEED RATE 100 E, DDA.
Pg26. “DATA INPUT” Press G00/G01. “X” 12.0 E, “Z” -30.5 E, FEED RATE 100 E, DDA.
Pg27. “DATA INPUT” Press G00/G01. “X” 12.0 E, “Z” -35.5 E, FEED RATE 100 E, DDA.
Pg28. “DATA INPUT” Press G00/G01. “X” 13.0 E, “Z” 25.0 E, FEED RATE 1200 E, DDA.
Pg29. “DATA INPUT” Press M05. (Spindle STOP) DDA.
Pg30. “DATA INPUT” Press G00/G01. “X” 13.0 E, “Z” 0.0 E, FEED RATE 1000 E, TOOL – No 2 E, SPINDLE – SPEED 150 E, DDA.
Pg31. “DATA INPUT” Press M03.
Pg32. “DATA INPUT” Press G00/G01. “X” 6.0 E, “Z” 2.0 E, FEED RATE 1200 E, DDA.

It is important to note that the “Length of Cut” on Pg33 is -14.5 because the “Start of the Cut” on Pg 32 is 2.0mm away from the front of the work piece. 14.5-2.0 leaves an actual “Length of Cut” of 12.5mm.

(Start of Screw Cutting).

Pg33. “DATA INPUT” Press G33. O/D (Outside Dia)=12.0, R/D (Root Dia)=9.85, Cut X=0.04, L-14.5, (Length of Cut), Pitch 1.75, (Thread Pitch), Starts 1, (Number of Starts), Tool 2, Speed 150. DDA.
This is an EXTERNAL thread because, the O/D is GREATER than the Root Dia. For an INTERNAL thread this would be reversed.

(End of Screw Cutting).

Pg34. “DATA INPUT” Press G00/G01. “X” 10.0 E, “Z” 3.0 E, FEED RATE 1000, T2. E, DDA.
Pg35. “DATA INPUT” Press G00/G01. “X” 13.0 E, “Z” 5.0 E, FEED RATE 1000 E, DDA.
Pg36. “DATA INPUT” Press M05. (Spindle STOP) DDA.
Pg37. “DATA INPUT” Press M02. (End Of Program).

F1 QUIT (To Leave Program Pages).
Green Screen display. “DATA INPUT” Press (8) GRAPHIC SIMULATION. E
BILLET SIZE? Diameter 30.0 E

(I have chosen a size bigger than the actual bar size so that the cut will be visible in the simulation)
Length (outside chuck) 44.0 E
Diameter (for drill size press D) else E to continue.

A simulated Chuck with your bar protruding will be shown on screen.
If you wish to increase the scale of this picture, “DATA INPUT” press the SINGLE UP ARROW key. (Multiple presses will increase the image further.)
If you wish to decrease the scale of this picture, “DATA INPUT”, press the SINGLE DOWN ARROW key.
To exit this section, add tools for simulation and to RUN simulation, “DATA INPUT”, E
The tools list/shapes will be displayed at the bottom of the Green Screen display.
Begin by pressing 0,1,2, etc until all tools you require are shown with a number below each tool. Press E
Run the “SIMULATION” which will be shown on the Green Screen display to show your program is safe and correct.
To RUN simulation, “MANUAL” Press Green START.
To QUIT simulation, “MANUAL” Press Red STOP.
You will now have returned back to the Main Menu on the Green Screen display.
Place part in chuck and tighten.
Press and release “EMERGENCY STOP” button to enter manual mode.
To move between the three settings below, “MANUAL” Press the HAND key and watch the display alter in the bottom right hand corner of the Green Screen display.
FAST FEED – Moves Very Quickly.
SLOW FEED – Moves More Slowly.
STEP FEED – Moves at 0.01m/m Increments Per Press.

Place R.H. turning tool in tool post.
Press Spindle “ON” (green button on “SPINDLE CONTROL” pad).
Continue pressing “+” key (“SPINDLE CONTROL” pad) to increase spindle speed to desired RPM, this will be displayed on the Green Screen display. (I am using an Aluminium bar of about 25.4mm diameter and about 63mm long to carry out this set-up and therefore have taken the spindle speed up to 1000 RPM).
Manually jog the tool to face off the end of the part in the chuck to allow accurate setting of the tools in a “Z” direction (in the direction of the chuck).
Manually jog the tool to turn a random diameter on the part in the chuck to allow accurate setting of the tools in a “X” direction (at 90 Degrees to the chuck).
Turn the spindle “OFF” (red stop button on “SPINDLE CONTROL” pad).
Jog X & Z away from the part in the chuck and remove the tool.

In order to leave this section, press red stop button on “MANUAL” pad.
You will now have returned back to the Main Menu on the Green Screen display.
Green Screen display. “DATA INPUT” Press (7) EXECUTE PROGRAM. E
Green Screen display. MANUAL OPERATION displayed on screen.
To LOCATE TOOL OFFSETS, “MANUAL” Press Red STOP.
TOOL OFFSETS Page now displayed.
“DATA INPUT” Press (1) SET TOOL OFFSETS. E
Tool No 0 (zero), E
Place TOOL 0 into the tool post. (Mine is a piece of steel in the shape of a small engineers square, pointing towards the chuck).
To move between the three settings below, “MANUAL” Press the HAND key and watch the display alter in the bottom right hand corner of the Green Screen display.
FAST FEED – Moves Very Quickly.
SLOW FEED – Moves More Slowly.
STEP FEED – Moves at 0.01m/m Increments Per Press.
Jog the tool up against the end of the turned bar in the chuck, in the Z direction, using “MANUAL” directional keys.
(Or, use the “SLIP” method. This requires the use of a known width “SLIP” which is slid in and out between the tool and the bar end whilst jogging the tool towards the bar, until it is considered a tight enough fit that it will not fall out under its own weight. This size is recorded but later you must return to the tool library to adjust the tool offsets to remove the “SLIP” width from the recorded sizes.)
To confirm this “Z” position in the offset library, “MANUAL” Press Red STOP. (The cursor will move from “Touch Z0 Plane” down to “Touch known X diameter”.)
Jog the tool to carry out the same procedure, but this time in the X direction, against the bar diameter.
To confirm this “X” position in the offset library, “MANUAL” Press Red STOP. (The cursor will move from “Touch known X diameter” down to “Key-In Dia”.)
KEY-IN DIAMETER: 25.4 E
Jog saddle away from bar in chuck, remove TOOL 0 from the tool post, place TOOL 1 into the tool post and begin the above process again.
You must start with, Tool No 1 E
Jog the tool up against the end of the turned bar in the chuck, in the Z direction.
To confirm this “Z” position in the offset library, “MANUAL” Press Red STOP.
Jog the tool to carry out the same procedure, but this time in the X direction, against the bar diameter.
To confirm this “X” position in the offset library, “MANUAL” Press Red STOP.
KEY-IN DIAMETER: 25.4 E

Jog saddle away from bar in chuck, remove TOOL 1 from the tool post, place TOOL 2 into the tool post and begin the above process again for this and subsequent tools.
Things to be aware of.

FIRST.
It is important to remember that when setting a Screw Cutting tool, a Centre Cutting tool, a Parting Off tool and a Left Handed Turning tool, that you will have to make adjustments to the offsets for these tools as they will NOT be cutting on the edge which you have set them off. For my Screw Cutting tool, I have measured the distance from the front face of the tool body to the centre line of the actual cutting point of the tool, set the tool off the front face of the tool body and then added that difference to the tool offset in the Tool Offset page. This will transfer the “Z” position for this tool to the actual cutting plane.

SECOND.
It is important to remember that when using one of these tools, as the cutting centre has moved away from the leading edge of the tool/tool holder, you MUST account for this if cutting up against a shoulder etc. Leave enough room for the front edge of the tool to move into this space without crashing your machine/job.

To QUIT TOOL OFFSETS, “DATA INPUT” E
REMOVE LAST SET TOOL AND WORK PIECE FROM CHUCK.
Now carry out a “DRY RUN”.
PRESS “F” TO START; AT PAGE 1 E

Now run the program using tools in the tool post but NO part in the chuck.
Machine runs up slowly, to continue, “MANUAL” Press Green START (sometimes more than once). Spindle will increase to program speed, then begin the program routine and end with a return to the tool change position.
Green Screen display. “DATA INPUT” Press (7) EXECUTE PROGRAM. E “MANUAL” Press Red STOP
Green Screen display “F” 1 E
Machine runs up slowly, to continue, “MANUAL” Press Green START. Spindle will increase to program speed, then begin the program routine and end with a return to the tool change position.

If you are satisfied there will be no accident, run it again, this time include the tools placed in the tool post and return the part to the chuck.
If you used the “SLIP” method, the tool should not touch the bar in the chuck as it should be the slip width away in both X & Z directions. I used a 0.5mm “SLIP”.
Green Screen display. “DATA INPUT” Press (7) EXECUTE PROGRAM. E
To LOCATE TOOL OFFSETS, “MANUAL” Press Red STOP.
TOOL OFFSETS Page now displayed.
“DATA INPUT” Press (2) EDIT TOOL OFFSET. E

I have had a re-think about adjusting all the tool offsets to comply with the ZERO tool, there is room for error if all tools are to be altered by the 0.50mm set piece. Instead, it will be far less complicated by just adjusting the ZERO tools offsets by -0.50mm in X and Z. This will bring ALL tools closer by 0.50mm.
T0 X -000.50 Z -000.50
T1 X 011.17 Z 042.62
T2 X 005.38 Z 038.46
When all tools lengths and diameters have been adjusted, “DATA INPUT” F to EXIT. With the tools offset page showing on the Green Screen display, Press “F” 1 E “MANUAL” Press Green START.

Run the program and you should now have a completed part which will need its sizes checking and any minor alterations made to each tools offsets in the TOOL OFFSETS to achieve the desired finished part.

To REMOVE more material from work diameter, INCREASE “X” figure in tool offset for that tool.
To move tool TOWARDS the chuck, INCREASE “Z” figure in tool offset for that tool.
To make alterations to the tool offsets, use the left, right, up, down SINGLE ARROW keys on the “DATA INPUT” pad.

NB. You must ONLY increase the “X” figure by HALF the amount you wish to remove from the bar diameter. i.e. To decrease the bar diameter by 1.0mm you must increase the “X” offset only by 0.5mm. This will remove 0.50mm per side, thus 1.0mm will be removed overall.

Remember to save your program if you wish to re-use it.

Post Reply