Horizontal Mill

[metalmilita]

Can anyone share some example MCAM9 Horizontal mill projects. I've ran VMC's for a long time and we just got in a horizontal. Never programmed one before just wanted to see how other do it and take notes. Also what do you recommend for drilling a 1/4 Dia. 12" deep blind hole in S-7 for a VMC.

 

 

Thanks for any help

[lanart]

I'm in the same boat. have a Haas EC-400 coming in a few weeks.

[Lars Christensen]

Dont have any examples to share, but the skinny is this.

draw everything up in Mastercam such as your tombstone, fixtures, travel distance, all your tools with you tool holder and spindle as a custom tool, so you can verify clearances. You will be using WCS to program the different sides of the tombstone. Side 0(side view) Side 90 (view#3) Side 180 (view#6) Side 270 (front view)

 

If you are going to use it for production I would recommends placing G54 at the center of your pallet and programing in G90 mode, then if you got everything drawend up correct Mastercam will take care of everything else.

 

If you are going to use the machine in a job shop inveriment you might find it easier having workoffsets placed on each side G54 G55 etc. you can get fancy and use G10 (Fanuc)in your program to dedicate the workoffsets.

 

HTH

Lars

[crazy^millman]

quote:

---

You will be using WCS to program the different sides of the tombstone. Side 0(side view) Side 90 (view#3) Side 180 (view#6) Side 270 (front view)

---

Sorry Lars but this statement is wrong. You will be using C & T Planes to Program the different sides of the tombstone. If you use WCS for each side then each side outputted as code will be A0. There are sample files for this type of programming in the sample files if you have the latest and greatest version or your latest disk from your dealer.

 

HTH

[Hardmill]

Both ways are correct, using your original WCS you can still

get the "A" axis output you want.

And you still utilize the WCS. A little more work but worth it.

 

 

PEACE

[crazy^millman]

Ok I have always used C-planes and T-planes. What all do you have to do to the post or WCS to get it to work and not give problems with multi-axis toolpaths??

 

I have always seen problems with Mastercam and Multi-Axis toolpaths when you start using more than one WCS.

[Guest CNC Apps Guy 1]

I'm with Ron. Lars' method may work, but Ron's method is the most common approach and is the easiest to implement.

 

Each operation will use the TOP WCS and T/C Planes for B0 will be Front, T/C Planes for B90 will be Right Side, T/C Planes for B180 will be Back, T/C Planes for B270 will be Left Side.

 

On the FTP in the following folder;

ftp://www.ppcadcam.com/Mastercam_forum/MC9_files/

there's an HMC Tombstone file. Check it out.

[Hardmill]

You need to use the original WCS in the planes box.

This will give you the correct rotations.

 

In this case B0 is the original.

Used to be a pain but edit common parameters handles it nicely now.

 

 

 

PEACE

[crazy^millman]

But that is not answering my question about multi-axis toolpaths. Do they play nice now with the different WCS???

 

I think you are creating more work than needed, but hey to each their own.

[Hardmill]

Actually it makes it easier to manipulate later on.

I have'nt seen any issues myself, but yes as you said i've heard

of these types of problems.

Most of the work ive done like this is surface machining.

And have not seen these issues, what toolpaths specifically ??

 

 

PEACE

[crazy^millman]

Curve 5 axis, 5 axis flowline, Advanced 5 axis Multi-surf in a 4 axis output. They in the past seem to do strange things so why risk it. I keep myself in the habit of doing it a way that eliminates possible problems I save myself the grief.

 

I have a part right now I am programming for a Hortzional that will be machined on all 5 sides using a Center support. If I am using what you say should use WCS for each side a see big problems. Where as if I use the One WCS and then My Cplanes/Tplanes to control my indexes I have no worries about maybe picking the WCS in the wrong place. I have done a lot of Single Part Hortzional Parts where the whole part rotates around Center. So know I use one method for parts of 4 faces of Tombstone and then a different Method for single parts. Sorry, but I like to keep it simples and use what I know is an easy method for my simple Brain to follow.

[Lars Christensen]

Thanks Ron, you are right I am not using WCS to machine the different sides, C and T plane is the way to go.

 

Thank you

Lars

[Tinhman]

I'm with Ron and CNC Apps Guy.

Wcs should stay on top and you can have as many as C and T plane (B0,B..., B90., B...) if you want.

Tinhman

X2 & Sw08

[metalmilita]

Thanks for all the help guys. As a matter of fact it is a 16i-MB Fanuc control Lars, could you tell me more about the G10 offsets. Also when i post out programs it outputs with A-Axis but i need B-Axis how do i change that in the mastercam post processor?

[cobra95kev]

metalmilita,

Which post are you using?

If you are still using a v9 post I think there should be a switch in the post you can change to differeniate between horizontal and vertical for rotary axis.

[metalmilita]

I'm using version 9.1. I've already switched it to horizontal but still doesn't work. Here's what i have in that section of the post proc.

 

# --------------------------------------------------------------------------

# Rotary Axis Settings

# --------------------------------------------------------------------------

vmc : 0 #0 = Horizontal Machine, 1 = Vertical Mill

rot_on_x : 2 #Default Rotary Axis Orientation, See ques. 164.

#0 = Off, 1 = About X, 2 = About Y, 3 = About Z

rot_ccw_pos : 1 #Axis signed dir, 0 = CW positive, 1 = CCW positive

index : 0 #Use index positioning, 0 = Full Rotary, 1 = Index only

ctable : 5 #Degrees for each index step with indexing spindle

use_frinv : 0 #Use Inverse Time Feedrates in 4 Axis, (0 = no, 1 = no )

maxfrdeg : 2000 #Limit for feed in deg/min

maxfrinv : 999.99#Limit for feed inverse time

frc_cinit : 1 #Force C axis reset at toolchange

ctol : 225 #Tolerance in deg. before rev flag changes

ixtol : .01 #Tolerance in deg. for index error

frdegstp : 10 #Step limit for rotary feed in deg/min

[Lars Christensen]

metalmilita,

Sorry I did not response sooner, there should be a section in your manual there cover the G10 function.

As of explaining it here on the forum, you would be much better of if Crazy Millman or CNC Apps Guy would explain it than me

[Rick Henrickson 65]

I agree with Ron the wcs top and c and t planes to handle the rotations is the way to go, verification is easier and I have never had a problem or a multi edit issue.

[metalmilita]

Still can't post out B-Axis movements only A-Axis. Is there something i can add to the post to accomplish this?

[Rick Henrickson 65]

how do you hae your wcs c and t planes set up?

[iowajim62]

metal,

quote:

---

Still can't post out B-Axis movements only A-Axis

---

look here in your post and change to B from A

HTH

code:

---

 # --------------------------------------------------------------------------

# Rotary Axis Settings

# --------------------------------------------------------------------------

# Typical Vertical

srotary "B" #Rotary axis prefix

vmc : 0 #0 = Horizontal Machine, 1 = Vertical Mill

rot_on_x : 2 #Default Rotary Axis Orientation, See ques. 164.

#0 = Off, 1 = About X, 2 = About Y, 3 = About Z

# Typical Horizontal

#srotary "B" #Rotary axis prefix

#vmc : 0 #0 = Horizontal Machine, 1 = Vertical Mill

#rot_on_x : 2 #Default Rotary Axis Orientation, See ques. 164.

# #0 = Off, 1 = About X, 2 = About Y, 3 = About Z

---

[crazy^millman]

Do you want the output to be in a B format. Like B135. If so go to the post and change the A to a B and that should take care of it for you. Do you have the question in the post set up for a Horizontal Machine??

 

Look here in the V9 post:

code:

---

# --------------------------------------------------------------------------

# Rotary Axis Settings

# --------------------------------------------------------------------------

vmc : 1 #0 = Horizontal Machine, 1 = Vertical Mill

rot_on_x : 1 #Default Rotary Axis Orientation ->

#0 = Off, 1 = About X, 2 = About Y, 3 = About Z

#Also check the setting of Post Numbered Question 164.

#164. Enable Rotary Axis button? y

#This must be set to 'y' to enable rotary!

rot_ccw_pos : 1 #Axis signed dir, 0 = CW positive, 1 = CCW positive

index : 1 #Use index positioning, 0 = Full Rotary, 1 = Index only

ctable : 5 #Degrees for each index step with indexing spindle

use_frinv : 0 #Use Inverse Time Feedrates in 4 Axis, (0 = no, 1 = yes)

maxfrdeg : 2000 #Limit for feed in deg/min

maxfrinv : 999.99#Limit for feed inverse time

frc_cinit : 1 #Force C axis reset at toolchange

ctol : 225 #Tolerance in deg. before rev flag changes

ixtol : .01 #Tolerance in deg. for index error

frdegstp : 10 #Step limit for rotary feed in deg/min

indextest : 0 #Index test variable used to output M60/M61 brake codes

 

scaxadrs A #Address for the rotary axis

scaxminus A- #Address for the rotary axis (signed motion)

---

HTH

[metalmilita]

I don't have the Typical Vertical and Horizontal Settings, or the rotary prefix. All I have is

 

# --------------------------------------------------------------------------

# Rotary Axis Settings

# --------------------------------------------------------------------------

vmc : 0 #0 = Horizontal Machine, 1 = Vertical Mill

rot_on_x : 2 #Default Rotary Axis Orientation, See ques. 164.

#0 = Off, 1 = About X, 2 = About Y, 3 = About Z

rot_ccw_pos : 1 #Axis signed dir, 0 = CW positive, 1 = CCW positive

index : 0 #Use index positioning, 0 = Full Rotary, 1 = Index only

ctable : 5 #Degrees for each index step with indexing spindle

use_frinv : 0 #Use Inverse Time Feedrates in 4 Axis, (0 = no, 1 = no )

maxfrdeg : 2000 #Limit for feed in deg/min

maxfrinv : 999.99#Limit for feed inverse time

frc_cinit : 1 #Force C axis reset at toolchange

ctol : 225 #Tolerance in deg. before rev flag changes

ixtol : .01 #Tolerance in deg. for index error

frdegstp : 10 #Step limit for rotary feed in deg/min

[Guest CNC Apps Guy 1]

You've GOT to have a variable assigning the address in theree somewhere. Look where all the letters are in the format statements... You know, where you find "F", "T", "S", etc..., look for the "B".

 

HTH

[iowajim62]

metal,

look here and change the A to B where it shows C axis position and Index position

code:

---

 # --------------------------------------------------------------------------

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

fmt T 4 t #Tool No

fmt T 4 first_tool #First Tool Used

fmt T 4 next_tool #Next Tool Used

fmt D 4 tloffno #Diameter Offset No

fmt H 4 tlngno #Length Offset No

fmt G 4 g_wcs #WCS G address

fmt P 4 p_wcs #WCS P address

fmt S 4 speed #Spindle Speed

fmt M 4 gear #Gear range

# --------------------------------------------------------------------------

fmt N 4 n #Sequence number

fmt X 2 xabs #X position output

fmt Y 2 yabs #Y position output

fmt Z 2 zabs #Z position output

fmt X 3 xinc #X position output

fmt Y 3 yinc #Y position output

fmt Z 3 zinc #Z position output

fmt A 11 cabs #C axis position

fmt A 14 cinc #C axis position

fmt A 4 indx_out #Index position

fmt R 14 rt_cinc #C axis position, G68

fmt I 3 i #Arc center description in X

fmt J 3 j #Arc center description in Y

fmt K 3 k #Arc center description in Z

fmt K 2 lead #Helical lead

fmt R 2 arcrad #Arc Radius

fmt F 15 feed #Feedrate

fmt P 11 dwell #Dwell

fmt M 5 cantext #Canned text

# --------------------------------------------------------------------------

---