Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

vtl md and post

Jeremy Herron@DBS Solutions™
 Share

Recommended Posts

Jeremy Herron@DBS Solutions™ Newbie

Jeremy Herron@DBS Solutions™

Posted
Posted

I have a mazak megaturn 900m which is a right turret vtl with live tooling. I currently program it just like a horizontal lathe with a modified mplmaster post. This is just fine for me but when we do setup sheets for the operators they are 90 degrees off. I have been trying to figure out how to make it look like a vtl on my screen while programming. I can get it to look right on the screen and all my X's and g2's and g3's post right for the turn work, but no matter what I have tried all my mill work comes out with negative x values. I know I am probably missing something stupid here. Anyone have any ideas?

Link to comment
Share on other sites
K2csq7 Newbie

K2csq7

Posted
Posted

Hi Jeremy...

I don't do any mill turn stuff.

 

Do the X values in the NCI look correct?

If you would like to create a quick file and send it my way I'd be happy to take a look, if you do, save the gcode as a txt file (good and bad) and send that too.

I have a stock mplmaster post, MD & CD I could use to play with.

 

Nothing I hate more than crickets...

  • Like 1
Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Jeremy,

 

Is the Machine Definition setup with the 'Vertical turret lathe' orientation (Machine Definition Manager > General Machine Parameters > Cplane, WCS, HTL/VTL Tab)?

 

Since you are using MPLMaster, that Post may or may not support the VTL Machine Components.

 

When you select the 'Vertical turret lathe' orientation switch, Mastercam will automatically re-map the planes to show the Lathe in the correct orientation. I suspect this is what is happening with your X values being incorrect.

 

Once you are using a properly defined VTL Machine Definition and Post (that reads the MD), you should get correct output. Keep in mind you will still want to use the +D+Z T/C Plane for programming. (But Mastercam will show the orientation correctly.)

 

When you use the "Top" graphics view with the VTL Machine selected, you will see that the part is shown to you in a Vertical orientation. 'Z' will now take the place of the Y Axis, and X+ will be on the Right side of the Z axis centerline. (so make sure your geometry is created on the right side of the axis centerline.

 

Your Tools will appear correctly for the setup sheets and Backplot and Verify will also be correct.

 

There is an existing MD/CD/PST combination for VTL Machines in X5. There is a Multi-Turret VTL Machine, and a Right Turret VTL Machine. You can probably save yourself a lot of time and trouble by using these existing files, and customizing the Post to your preferences.

 

If you click on the help button in the Cplane, WCS, HTL/VTL Tab of the MDM, there are several help entries that describe how to setup a VTL Machine Definition. Try reading through those sections and see if that helps you make sense of it.

 

I can't help you with the MPLMaster Post, as it isn't a CNC Software Post. If you choose to start fresh with our 'Generic Fanuc 4X MT_Lathe' post, I can answer your questions about how to configure that post for your machine.

 

Hope that helps,

  • Like 1
Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Yes, It is showing that left of the Centerline is X Negative. If you draw your geometry on the right side of Centerline, it will output as X+ Coordinates. When you select a Tool, make sure you have the tools setup correctly. (I always use "Draw Tool" when setting up a Lathe Tool.)

 

Keep in mind: you can change the Properties for your VTL Turret Component, including the orientation. Set the turret axis to the axis it actually rotates about, and set the other properties. The only things you really need to worry about are min/max live tool speed, Axis of Rotation, Index Axis, and Indexing Method.

 

Also, you need to go into "Axis Combinations", and then set the Home Position. Then when you Backplot it will show the tool retracting to the home position for tool changes.

Link to comment
Share on other sites
Jeremy Herron@DBS Solutions™ Newbie

Jeremy Herron@DBS Solutions™

Posted
  • Author
Posted

Okay, my tools are set correctly and show on the screen right. I have a simple face path and turn path and c-axis face drill tool path. my posted code is:

 

 

 

TOOL - 1 OFFSET - 1)

(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG-432)

G28 U0. W0.

G0 T0100

G0 T0101

G97 S76 M03

G0 X-10.1 Z.1

G50 S1000

G96 S200

G99 G1 Z0. F.01

X.06

Z.1

T0100

G28 U0. W0. M05

M01

(TOOL - 1 OFFSET - 1)

(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG-432)

G28 U0. W0.

G0 T0100

G0 T0101

G97 S82 M03

G0 X-9.2961 Z.0707

G50 S1000

G96 S200

G1 X-9.4375 Z0. F.01

G3 X-10. Z-.2813 K-.2813

G1 Z-1.

X-10.1414 Z-.9293

T0100

G28 U0. W0. M05

M01

(TOOL - 5 OFFSET - 5)

( 1/4 SPOTDRILL)

( C-AXIS FACE DRILL )

G0 T0505

M23

G0 G54 X5. Z1.

C180.

G97 S1069 M52

G83 Z-.1 R.1 Q1. F1.07

C225.

C270.

C315.

C360.

C405.

C450.

C495.

G80

G28 U0. W0. H0. M55

T0500

M30

%

 

 

 

 

The "x" values in the turn work are negative, the "x" values in the c-axis tool path is correct, but it says "c180." for my "c0." hole

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Jeremy,

 

In your Generic Fanuc 4X MT_Lathe Post, you need to change the following:

 

dia_mult : -2 (Change from '2' to '-2')

 

Changing this variable to a minus value will reverse the X coordinate output.

 

You may also need to set a rotation value for this variable:

 

c_shift : 0

 

If your C axis coordinates are 180 degrees off, then use '180' or '-180'. That should fix the C Axis values...

Link to comment
Share on other sites
Jeremy Herron@DBS Solutions™ Newbie

Jeremy Herron@DBS Solutions™

Posted
  • Author
Posted

I was right. I just had to make sure. It appears right on my screen and the "C" values are correct, but...

 

(TOOL - 5 OFFSET - 5)

( 1/4 SPOTDRILL)

( C-AXIS FACE DRILL )

G28 U0. W0.

G0 T0500

G0 T0505

M23

G0 X-5. Z1. ---------------------------------- this should be be "X5."-----------------------------

C0.

G97 S1069 M52 ------------------------- this should be m53 as well _____________ fissed

G83 Z-.1 R.1 Q1. F1.07

C45.

C90.

C135.

C180.

C225.

C270.

C315.

G80

T0500

G28 U0. W0. H0. M55

M30

 

 

any ideas?

 

 

 

thanks again

Link to comment
Share on other sites
K2csq7 Newbie

K2csq7

Posted
Posted

Hi Jeremy, I was out for a week or so with the power outage (took em 7 days to get mine back on and I live in a pretty well populated area) & had a new baby at the same time... are you just rubbing in the fact that I don't have X6 yet? :rolleyes: Your zipped file is .MCX-6... If you save it as an old school X5 file, I'd be happy to take a look. I don't do any Mill/Turn work but am always up for a challenge..:D

Link to comment
Share on other sites
K2csq7 Newbie

K2csq7

Posted
Posted

Hi Jeremy, I didn't have much luck playing with the post....

couple questions.... the setting for the c axis in the MD has the zero position at -X.... I cant find where in the post to change that... changing it in the MD had no effect...

Also the drill backplots on the left side.... I was expecting to see it on the right.... with the lathe tools.

 

I will have some more time tomorrow to look into it :D

Link to comment
Share on other sites
Jeremy Herron@DBS Solutions™ Newbie

Jeremy Herron@DBS Solutions™

Posted
  • Author
Posted

The "c_shift" variable in the post set to 180 makes the c numbers right, otherwise my firts hole is at "x-5 c180." , and in backplot even though it is on the left side it says it is at "x+2.5" which is right. I am perplexed. I even tried setting the c shift 0 and picking the 180 hole as my first hole and it has no effect. :head scratching:

Link to comment
Share on other sites
Mgrenier Newbie

Mgrenier

Posted
Posted

Jeremy,

 

You need to find this section in you post and adjust it to your needs. This is what we have and dia_mult = 2.

 

#Machining position turret/spindle settings
# Switch strings based on turret position top/bottom-left/right and cut type.
# Turret position is based on the Mastercam settings (see lathtype).
# Strings are re-assigned for output in the routine psw_str_mult.
# The string variable sw_string holds the place position value to determine
# how to assign the strings.  Planes are relative to the view from Mastercam.
# Assign the 17 digit string following the alpha columns below:
# A - C axis, 1 = axis winds, 2 = axis signed, 3 = indexer
# B - Spindle direction, 0 = normal, 1 = reverse
# C - Plane 0 arc/comp, 0 = normal, 1 = switch
# D - Plane 1 arc/comp, 0 = normal, 1 = switch
# E - Plane 2 arc/comp, 0 = normal, 1 = switch
# F - Plane 0, 0 = G17, 1 = G19, 2 = G18
# G - Plane 1, 0 = G17, 1 = G19, 2 = G18
# H - Plane 2, 0 = G17, 1 = G19, 2 = G18
# Decimal (required)
# I - Plane 0, X axis, 0 = normal, 1 = switch sign from basic
# J - Plane 0, Y axis, 0 = normal, 1 = switch sign from basic
# K - Plane 0, Z axis, 0 = normal, 1 = switch sign from basic
# L - Plane 1, X axis, 0 = normal, 1 = switch sign from basic
# M - Plane 1, Y axis, 0 = normal, 1 = switch sign from basic
# N - Plane 1, Z axis, 0 = normal, 1 = switch sign from basic
# O - Plane 2, X axis, 0 = normal, 1 = switch sign from basic
# P - Plane 2, Y axis, 0 = normal, 1 = switch sign from basic
# Q - Plane 2, Z axis, 0 = normal, 1 = switch sign from basic
use_only_tl : 0     #Use only Top turret/Left spindle settings (below) for
                   #all Mastercam turret/spindle selections
                   #When configuring for multi-spindle/turret set to 0

#Columns-       ABCDEFGH.IJKLMNOPQ #Turret/Spindle            #Path Type
scase_tl_c1  : "10000222.100100100"  #Top turret/Left spindle, Turning cut
scase_tl_c2  : "10000012.000000000"  #Top turret/Left spindle, Right Face cut
scase_tl_c_2 : "10110012.000000000"  #Top turret/Left spindle, Left Face cut
scase_tl_c3  : "10010102.000000000"  #Top turret/Left spindle, Cross cut (cuttype = 3)
scase_tl_c3r : "10001102.000000000"  #Top turret/Left spindle, Reverse Cross cut (cuttype = -3)
scase_tl_c4c : "10000222.000000000"  #Top turret/Left spindle, Y axis subs. Cycle
scase_tl_c4  : "10000122.000000000"  #Top turret/Left spindle, Y axis subs.
scase_tl_c5  : "10000222.000000000"  #Top turret/Left spindle, Multisurf Rotary

#Columns-       ABCDEFGH.IJKLMNOPQ
scase_bl_c1  : "10000222.100100100"  #Bottom turret/Left spindle, Turning cut
scase_bl_c2  : "10000222.000000000"  #Bottom turret/Left spindle, Right Face cut
scase_bl_c_2 : "10110222.000000000"  #Bottom turret/Left spindle, Left Face cut
scase_bl_c3  : "10010222.000000000"  #Bottom turret/Left spindle, Cross cut (cuttype = 3)
scase_bl_c3r : "10010222.000000000"  #Bottom turret/Left spindle, Reverse Cross cut (cuttype = -3)
scase_bl_c4c : "10000222.000000000"  #Bottom turret/Left spindle, Y axis subs. Cycle
scase_bl_c4  : "10000222.000000000"  #Bottom turret/Left spindle, Y axis subs.
scase_bl_c5  : "10000222.000000000"  #Bottom turret/Left spindle, Multisurf Rotary

#Columns-       ABCDEFGH.IJKLMNOPQ
scase_tr_c1  : "10000222.000000000"  #Top turret/Right spindle, Turning cut
scase_tr_c2  : "10000012.000000000"  #Top turret/Right spindle, Right Face cut
scase_tr_c_2 : "10110012.000000000"  #Top turret/Right spindle, Left Face cut
scase_tr_c3  : "10010102.000000000"  #Top turret/Right spindle, Cross cut (cuttype = 3)
scase_tr_c3r : "10001102.000000000"  #Top turret/Right spindle, Reverse Cross cut (cuttype = -3)
scase_tr_c4c : "10000222.000000000"  #Top turret/Right spindle, Y axis subs. Cycle
scase_tr_c4  : "10000222.000000000"  #Top turret/Right spindle, Y axis subs.
scase_tr_c5  : "10000222.000000000"  #Top turret/Right spindle, Multisurf Rotary

#Columns-       ABCDEFGH.IJKLMNOPQ
scase_br_c1  : "10000222.000000000"  #Bottom turret/Right spindle, Turning cut
scase_br_c2  : "10000222.000000000"  #Bottom turret/Right spindle, Right Face cut
scase_br_c_2 : "10110222.000000000"  #Bottom turret/Right spindle, Left Face cut
scase_br_c3  : "10010222.000000000"  #Bottom turret/Right spindle, Cross cut (cuttype = 3)
scase_br_c3r : "10010222.000000000"  #Bottom turret/Right spindle, Reverse Cross cut (cuttype = -3)
scase_br_c4c : "10000222.000000000"  #Bottom turret/Right spindle, Y axis subs. Cycle
scase_br_c4  : "10000222.000000000"  #Bottom turret/Right spindle, Y axis subs.
scase_br_c5  : "10000222.000000000"  #Bottom turret/Right spindle, Multisurf Rotary

 

HTH

 

 

Link to comment
Share on other sites
K2csq7 Newbie

K2csq7

Posted
Posted

I got the spindle and X codes to come out right....

scase_tl_c2 : "10000012.100000000" #Top turret/Left spindle, Right Face cut

 

changing this line here did that for me yesterday, but since the drill showed up on the left of centerline I convinced myself that was not the right way to do it.

I started looking into the MD to try to get the drill to backplot on the same side as the turning tools...

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...