boring bar retract

[Thoob]

I'm cutting a key on a lathe right now but I'm trying to make it retract to the same spot every time. Heres the thing, When I get to the end of the key on z, I need the tool to clear the top of the key way by .02. (Tool cannot rub at all on the way back) I can only go .02 as I am in a very tight bore and my tool is very close to the edge. That being said, if I set it to .02, it only retracts incrementally instead of to the absolute. Am I able to change this?

[Guest]

Can you draw the leg of the motion you need and add it as part of the cutting chain?

 

Then change your Lead out direction to pull back instead of off

[K2csq7]

I would just draw & chain EXACTLY what you want, shut off lead in/out, then use a finish path with ref points.

 

But thats what I do all the time....

PITA, but no surprises......

[Thoob]

I can do that yes. I just thought there was a way to do an absolute retract. Thanks.

 

edit. That is not working for me. Mastercam thinks it is removing material on the diameter so it thinks the material is gone. I can't get it to retract out no matter if I add a line or not? Why is there not such a simple option to retract in absolute? lol.

[Thoob]

Anyone willing to take a look at the file? I can email it to you.

[K2csq7]

[email protected]

[JerryBenoit]

Thoob,

 

No I do not believe there is. What I have done in the pass is write a macro on the machine to do what you are looking for. I tailored it simalar to a G76 thread cycle retracking in the X axis to a safe point. But if you are pressed for time you may want to do what John mentioned used the finish cycle on lead in out. Set the Finish stepover to your desired depthof cut and the Number of passes to what you need to finish the keyway. After you post it out edit the code to retrack in X the same everytime.

 

Jerry

[Thoob]

sent.

[NOTW Programmer]

Anyone willing to take a look at the file? I can email it to you.

[email protected]

[Thoob]

I got it to work with what Paris said. Now I have a bigger issue. My lathe memory capacity is 19.5 kilobytes (not a typo,very limited). The program posts out at 22kb. There are lots of these parts so splitting the program is not an option. I need to get the file size lowered somehow. When I did it in roughing mode, the program was not over the limit but since I have added the extra line, its over. Any ideas how I can fix this?

I probably should have mentioned this earlier but the key is on a tapered bore so the lathe is moving on x and z simultaneously.

[K2csq7]

I am looking at the file, for another crack at explaining this, he basically has a bunch of multi-passes (229 of them spaced .001 apart) that he wants all to retract to the same point.

I don't think that's an option.

 

What I would suggest is to create a lathe finish pass that would be the first pass the tool will make, then transform that path .001 in X, 229 times. set the transform to create new ops, then select all of the new ops, edit selected ops, and add a retract ref. point. The 229 ops will still have the lead out of the original op, so that will have to be set up before the transform is done.

Transform method will be translate between points, from point will be 0,0,0,..... to point will be 0,.001,0.

 

What do you think?

 

Edit: I suggest setting the number of instances to 10 or 20 until your sure your getting what you want. (My computer is slow)

 

Retracts to the newly selected point will be rapid (.02 lead out is still feed)..... you can get the coordinates of the retract point by backplotting the op to be transformed.

[JerryBenoit]

Do you enter a groove at the end of the Keyway? If so can you use a G77 or G90 can cycle (depending on what G code system on fanuc controls).

 

Jerry

[Mick]

You could chain each pass, then click to a retract point at the end, then use a reference point. So the order of chaining would be (and this is how it would look in the chaining manager window):

 

chain

 

point

 

chain

 

point

 

chain

 

point

 

etc etc

 

The point is the same position every time.

 

I've doen this before for broaching a keyway on a lathe. Worked a treat. If you want the MCX-6 file, just send me your email address and I can email it through

[Mr. M]

I've done the broaching in an Okuma using a LAP cycle, but it could also be done easily in a macro. Both would give you a smaller file size.

[Zoffen]

Here's my gift to the party!

Broaching macro!

 

Use at own risk! Written for a Mazak Matrix T Control, 3 axis lathe.

Probably need to change the backoff moves ( the incemental moves) smaller and backoff amount #111 to a smaller number but should work.

Best thing to do is to make this a G-code Macro so u can call it when ever you want!

 

Also i attached my cheat sheet for macro variables to help clarify what each value is

I was thinking of adding z (well actually x in this case) level multipasses (with y axis) so you could broach a larger keyway with a smaller broach

 

Feel free to copy and improve!

Macros are fun!

 

O0001(Broaching)
(-----------Notes------------)
(Broaching Macro For Mazak Matrix T)
(Call Desired Tool Prior To Running Macro)
(Written By: Zack O.)
(V1.0 - 7/24/2012)
(This is a broaching macro for a 3 axis(C) Lathe)
(Provide all necesary info and the macro will)
(Calculate if the broach can fit and alarm out if not possible with parameters)
(Uses Rough and finish Feed Rates)
(You can restart where you left off by block deleteing where specified)
(User specified X Radial Clearance amount from start of broaching)
(-----Variables--------)
#101=.160  (Width of Broach)
#102=.520  (Thickness of broach)
(Measured from flat of broach to bottom of holder)
#103=-1.5  (Broach end Z Position)
#104=.625  (Start Hole Dia)
#105=.750  (Nominal Broach depth)
(Measured from flat to bottom of hole opposite)
#106=.025  (Depth of Cut)
#107=200.  (Rough Feed-IPM)
#108=100   (Finish Feed-IPM)
#109=0     (C axis position of broaching)
#111=.05   (X Radial Backoff Amount from first cut- CLEARANCE)
(-Calculated-#1= X Dia Max Depth of Broach Position-)
(-Calculated-#2= X Dia Start of broaching-)
(-Calculated-#3= Radius of start hole-)
(-Calculated-#4= Half of width of keyway-)
(-Calculated-#5= Radius of Start hole squared-)
(-Calculated-#6= Radial distance to broach fist pass position-)
(-#199 holds current X pass position of broach-)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(----------------------)
(-----Calculations-----)
(General Calculations)
#3=#104 / 2 
#4=#101 / 2
#5=#3 * #3
(Calculate X Dia End Position)
#1=[[#105-#104]*2]+#104  ([[broach Dia minus start diameter] times 2] plus start hole dia= X Diameter value of final broach depth)
(Calculate X Dia start position)
#7=#5-[#4 * #4]
#6=SQRT[#7]
#2=#6+#6
(Calculate if Broach can fit in hole with #111 Backoff/Clearance Amount)
#8=#6+#3
#9=#111/2
#10=#8-#9
(Check to see if broach will fit in hole)
IF[#102GT#10] GOTO1001
(Program Motion)
G53.5
T0404.00
G98
M200
C#109
G0 Z1.0
M01
(Activate Block Delete)
(To Start At Last Position)
\#199=#2
X#199
WHILE[#199LT[#1-[#106*2]]] DO1
M01
#199=#199+[#106*2]
X#199
G01 Z#103 F#107
G0 W.025 U-.050
X#2-[#111*2]
Z1.0
END1
(Finish Pass)
M01
X#1
G01 Z#103 F#108
G0 W.025 U-.050
X#2-[#111*2]
Z1.0
M202
G99
M99
(-----Alarms------)
N1001 #3000= 101 (TOOL#TOO#LARGE)
M99

 

ya'll have fun now!

[GoetzInd]

Macros are fun!

 

[Thoob]

I was able to get it lower. My depth was about .06 too deep as the drawing had 2 dimensions. of course I picked the wrong one, lol. Anyway with that many lines removed, it fit in the memory. On another good note, I was told by the manufacturer that I could run off the memory card which is 1GB. This helped a lot. I appreciate all the help fellas. Take care.