Live Tooling Post For Haas ST-0

[Mastercam Rookie]

HI everyone,

 

Im going to see if i can get some help with my post processor file. Im currently running a "c-axis toolpath" in mastercam for "cross contour" and "cross drill", I have all the tool offsets set up in the hass st-10 but for some reason "c-axis toolpath" for "cross contour" and "cross drill" is not engaging, Im running to diffeent "NC Files" because I only have two Radial Live Tools. So I can only run two live tooling programs at a time. and to let you guys know im using the "GENERIC HAAS SL 4X MT_LATHE.LMD" post processor I also tried the "LATHE DEFAULT.LMD" but that one wasnt even generating the m-code "M154" to even engage the c-axis. Im pretty sure I dont even have the right post. but if somene could help me with the post or even explain it to me on how to fix mine so it would post right it would be highly appreciated. Oh and Im making a "Tap Wrench" so who ever can really help me out Ill mail them one!

 

So the first program you will see is (SETUP3) has two drill process ( 1/8 SPOTDRILL) and ( 3/8 DRILL)

And the Second program you will see is (SETUP4) has two drill process ( 1/4 FLAT ENDMILL) and ( 1/2 FLAT ENDMILL)

%

O0001

(SETUP3)

(DATE=DD-MM-YY - 18-05-14 TIME=HH:MM - 16:08)

(MCX FILE - C:\USERS\CNC\DESKTOP\TAPWRENCH\TAPWRENCHTEST101.MCX-7)

(NC FILE - C:\USERS\CNC\DESKTOP\SETUP3.NC)

(MATERIAL - ALUMINUM INCH - 6061)

G20

(TOOL - 4 OFFSET - 2)

( 1/8 SPOTDRILL)

(C-AXIS SPOT DRILL)

G00 T0402

G19

M154

G00 G54 X1. Z-2.75

C90.

G97 S2139 M51

G83 X.2 R.7 Q0. F1.03

G80

G00 Z-2.75

G28 U0. V0. W0. H0. M55

T0400

M01

(TOOL - 5 OFFSET - 4)

( 3/8 DRILL)

(DRILL)

G00 T0504

G19

G00 G54 X1. Z-2.75

C90.

G97 S1426 M51

G83 X-.9253 R.7 Q.1 F4.11

G80

G00 Z-2.75

G28 U0. V0. W0. H0. M55

T0500

M30

%

 

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

 

%

O0001

(SETUP4)

(DATE=DD-MM-YY - 18-05-14 TIME=HH:MM - 16:44)

(MCX FILE - C:\USERS\CNC\DESKTOP\TAPWRENCH\TAPWRENCHTEST101.MCX-7)

(NC FILE - C:\USERS\CNC\DESKTOP\SETUP4.NC)

(MATERIAL - ALUMINUM INCH - 6061)

G20

(TOOL - 4 OFFSET - 4)

( 1/4 FLAT ENDMILL)

(CONTOUR HOLE)

G00 T0404

G19

M154

G00 G54 X1. Z-2.8438

C90.

G97 S2139 M51

X.7

G98 G01 X.3 F6.42

Y-.0466 Z-2.7917

G2 Y-.0625 Z-2.75 R.0625

Y0. Z-2.6875 R.0625

Y.0625 Z-2.75 R.0625

Y.0466 Z-2.7917 R.0625

G01 Y0. Z-2.8438

X.1

Y-.0466 Z-2.7917

G2 Y-.0625 Z-2.75 R.0625

Y0. Z-2.6875 R.0625

Y.0625 Z-2.75 R.0625

Y.0466 Z-2.7917 R.0625

G01 Y0. Z-2.8438

X-.1

Y-.0466 Z-2.7917

G2 Y-.0625 Z-2.75 R.0625

Y0. Z-2.6875 R.0625

Y.0625 Z-2.75 R.0625

Y.0466 Z-2.7917 R.0625

G01 Y0. Z-2.8438

X-.3

Y-.0466 Z-2.7917

G2 Y-.0625 Z-2.75 R.0625

Y0. Z-2.6875 R.0625

Y.0625 Z-2.75 R.0625

Y.0466 Z-2.7917 R.0625

G01 Y0. Z-2.8438

X-.5

Y-.0466 Z-2.7917

G2 Y-.0625 Z-2.75 R.0625

Y0. Z-2.6875 R.0625

Y.0625 Z-2.75 R.0625

Y.0466 Z-2.7917 R.0625

G01 Y0. Z-2.8438

X-.7

Y-.0466 Z-2.7917

G2 Y-.0625 Z-2.75 R.0625

Y0. Z-2.6875 R.0625

Y.0625 Z-2.75 R.0625

Y.0466 Z-2.7917 R.0625

G01 Y0. Z-2.8438

G00 X1.

G00 Z-2.8438

G28 U0. V0. W0. H0. M55

T0400

M01

(TOOL - 1 OFFSET - 1)

( 1/2 FLAT ENDMILL)

(CONTOUR)

G00 T0101

G19

G00 G54 X1. Z-2.0625

C90.

G97 S1069 M51

X.7

G01 X.5 F6.42

Z-3.4375

G00 X1.

G55 X1. Y0. Z-2.0625 C270.

X.7

G01 X.5

Z-3.4375

G00 X1.

G00 Z-3.4375

G28 U0. V0. W0. H0. M55

T0100

M30

%

[GIZMO 21]

REALY!!!!!!!!!.YOU WANT A POST FOR A TAP WRENCH?.you better read the forum rules.

 

 

http://www.emastercam.com/forum-guidelines/

[Mastercam Rookie]

REALY!!!!!!!!!.YOU WANT A POST FOR A TAP WRENCH?.you better read the forum rules.

 

 

http://www.emasterca...rum-guidelines/

 

Ok, I edited the forum...but Im a student and are school dosent have a proper post for the ST-10 for live tooling and also dosent know how to run it, im the only one close enough running the live tooling. just trying to make a part with live tooling so I can show the other students...but it ok I dont think everybody wants a tap wrench

[crazy^millman]

Let me see if I can help out here. Many of us are hard working people who earn a living using this software and sometimes people come in there askign for a $XXXX or $XXXXXX cost post for free. Either they are to cheap to go out and get it or they have an illegal seat of software. Some know it alls love to make claims how other software give you this for free though that is not the case, WHY Vericut, ICAM and NC Simul all have healthy business because of the lack of posts many CAM Software's lack Mastercam included. There is an educational forum and had your question been posted in there and had you started out your 1st post with what you included in your 2nd post might have got a totally different answer from the start. One of my 1st projects back in the mid 80's when I took machine shop in school was use a hacksaw to cut off a piece of 1" x 1" Square stock and make a perfect 1" block, with at least a 16 finish only using hand tools. I an one other student were the only ones to get A's. I think I achieved a 2 finish though we could never really confirm it.

 

Your toolpath is physical impossible on that machine unless it has a Y axis. You need to up and down movement of the Y axis to create that shape. C axis toolpaths are just that they take the center line of the turning axis and use it to pivot the part to get to other palces you need items to be flat or with cross holes or features. The area for a tap is normally a V and the mating part is another V as thew handle is tightened down the to V's close and grab the squares on the top fo the tap to transfer the force from the handle which gives leverage to the tap using Physics and goes back to some know equations. I think Mastercam is not telling you it is not possible, but is breaking it up because of some other possible issues. #1 You could have a bad NCI name for each of the operations. You could have also en error going on it is not alerting you to that is also preventing it to post as once since what you are trying to machine is not physically possible and the bets you could hope to obtain is a cheat, which in my humble opinion would defeat the purpose of the exercise.

 

What are some possbile suggestions to help you get this made?

#1 if you had a Y axis then make a normal milling toolpath using the correct T-C Plane with a small enough radius tool. Take a file and make the corner small enough for the size tap you want to fit in it, or drill a small hole to make a radius to allow thee square corner to fall into it.

#2 Due a true manufacturing study and do it in several different capable machines. Also another trick is to take a taper ball endmill with a .015R and set the part up an a certain angle and then cut the walls with the taper ball endmill that is the inverse of the angle you have set it up at to create the perfect 90 degree angle you are looking for. It is possible, but that is one I want you and your class to figure out.

#3 Make a broach you can run on the C axis lathe with the C axis Spindle Locked and then step it over .002 to .003 at a time and cut the square corner you need with a broach. A broach is like a chisel for metal. Or course the material used has to be stronger than the material you are cutting.

 

Hopefully this is a full lesson in the manufacturing of a item that is taking you through metallurgy. The process of using a certain metal that was designed for the purpose you are intending to use it, also a study in Engineering. How is that you might ask, well an Engineer has to figure al of this out and many CNC Machinist, Programmers and just regular Machinist and Tool and Die Makers and hands on Engineers maybe more in every sense of the word sicne we use our hands to get it made and not read or see how it is made. No we can make the ideas they have and understand why or where it will most likely fail well before they even understand why? Why the metal acts the way it does and why the certain temperature will turn it into glass in the sense it is very brittle and then once it is tempered or annealed it is not as hard, but is strong. How if you use similar steels in certain situations when threads are involved you will create a gall situation and the metal will weld itself together. Why certain metals are used for their wear properties and others are used for their memory and yet how the plasticity other metals have helps them in other situations. You have a wonderful road ahead of you and I got started like you wanting to help my fellow classmates as I got something I would share and help them. I use to sharpen tools for my classmates $1 a tool and most weeks that paid my lunch and gave me a little spending money while I was working my 3 jobs. You did not say where you were, but if you are in Southern California let me know the school and I will be glad to stop by and help you and your class for a day no charge, just be glad to pass one something to help you on your way. All I would ask is 25 years from now you pass it on to others like I pass it on to you.

[Mastercam Rookie]

Thanks for you example

[Rocketmachinist]

I will help throw you a small bone, but its just to help you understand what the machine is looking for to use live tooling.

 

G00 T0402

G19

M154

G00 G54 X1. Z-2.75

C90.

M133 P2139 (it is a live tool callout and spindle speed must be called out with a p value)

G98 (needed bacuse the lathe uses ipr and milling requires ipm)

G83 X.2 R.7 Q0. F1.03 (this line will not work at all haas lathes have no caned cycles for live tooling except for tapping- go figure but they would be

(G195 LIVE TOOLING VECTOR TAPPING (X,F)

(G196 LIVE TOOLING VECTOR TAPPING REVERSE (X,F)

G80 (not needed if you don't have canned cycles)

G00 Z-2.75

G28 U0. W0. M135 (no H0 its not a mill amd no V0 unless you have a y axis)

T0400 (I never understood this line but people like putting it in their post anyways. My post doesn't have it and it doesn't make a difference.)

 

That should tell you enough to get yourself started.