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:

need help with post editing

jeff85

By jeff85,
in Educational Forum

 Share

Recommended Posts

jeff85 Newbie

jeff85

Posted
Posted

I just update my post for my uni project from v9 to x2.

but i got some problem with it

this is the old v9 generate

G0 T0101

G18

G97 S3600 M03

G0 X24. Z0. M8

G50 S3600

....

 

and this is from the updated

G28 U0. Y0. W0. <<<<<

G50 X250. Y0. Z250. <<<<<

G0 T0101

G18

G97 S3600 M03

G0 X24. Z0. M8

G50 S3600

 

I'm really experienced in updating post. can anyone help me where is the "<<<<<" comes from?

 

thank you,

jeff

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Hi Jeff,

 

Most posts are setup with 'switches' that allow you to enable/disable different features in the code being output.

 

For Lathe posts, there is usually an option to enable "G50 home positioning".

 

That is what you are seeing in your new code.

 

This output is typically enabled/disabled with Misc. Integer #1 in the toolpath.

 

Click on the 'Misc. values' button on the Toolpath parameters page of your operation.

 

What does the text for Misc. Integer # say, and what is the value.

 

Typically you'll see something like this at the top of the post:

 

code:
# Following Misc. Integers are used:

#

# mi1 - Work coordinate system: (home_type)

# -1 = Reference return / Tool offset positioning.

# 0 = G50 with the X and Z home positions.

# 1 = X and Z home positions.

# 2 = WCS of G54, G55.... based on Mastercam settings.

What is the "Value" for Misc. Integer #1?

 

I'm guessing it is defaulting to '0' which is giving you the 'G28 and G50' lines of code...

Link to comment
Share on other sites
jeff85 Newbie

jeff85

Posted
  • Author
Posted

I just checked it and the value is 0.

 

MILL/TURN FUNCTIONS SUPPORTED BY THIS POST #######

#

# This post supports Generic Fanuc code output for mill/turn lathes.

# It is designed to support the features of Mastercam Mill V8.

#

# Following Misc. Integers are used:

#

# mi1 - Work coordinate system: (home_type)

# -1 = Reference return / Tool offset positioning.

# 0 = G50 with the X and Z home positions.

# 1 = X and Z home positions.

# 2 = WCS of G54, G55.... based on Mastercam settings.

#

# mi2 - Absolute or Incremental positioning at top level

# 0 = absolute

# 1 = incremental

#

# mi3 = Select G28 or G30 reference point return:

# 0 = G28, 1 = G30

#

#mi4 = Canned conversion cycle type selection:

# Mill-

# Activates milling axis conversation canned cycles (G107 or G112).

# 1 or -1 activates the cycle, the path continues until next entry is

# zero, sign switches (1 to -1) forces g113 at null toolchnge, the

# cycle changes or the tool changes.

 

Could I know what should i change?

Link to comment
Share on other sites
  • 2 weeks later...
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

To set the defaults for the MI and MR values, you first need to "associate" your post with your control defintion.

 

You may have already done this, to check and see if you have, go into the post and scroll all the way to the bottom. There should be an entry there for each control definition that the post has been associated to. For example, in one of my posts I've got the following sections (each one has defaults listed underneath the control definition callout):

 

code:
[CTRL_MILL|MPMASTER]

.

.

.

 

[CTRL_MILL|HAAS_VF4_4_AXIS_MPMASTER_VERTICAL]

Each section has defaults for the different settings....

 

code:
[CTRL_MILL|HAAS_VF4_4_AXIS_MPMASTER_VERTICAL]

[misc integers]

1. ""//2

2. "Abs/Inc, top level [0=ABS,1=INC]"

3. ""

4. "Safe Index [0=Off,1=On]"

5. ""

6. "Unit/Rev Feed (G95) [0=No,1=Yes]"

7. ""

8. ""

9. "Lock on First WCS [0=No,1=Yes]"

10. "M00 before operation [0=No,1=Yes]"

[misc reals]

1. "HS [1=G08,2=AICC,3=HPCC,4=Mazak]"

2. "Accel/Decel Value [0=No output]"

3. ""

4. ""

5. ""

6. ""

7. ""

8. ""

9. ""

10. ""

[simple drill]

1. "G81/G82 - Drill/Counterbore"

3. "Dwell - G82"

7. ""

8. ""

9. ""

10. ""

11. ""

[peck drill]

1. "G83 - Peck Drill"

3. ""

9. "Minimum peck"

10. ""

11. ""

[chip break]

1. "G73 - Chip Break"

3. ""

8. ""

9. ""

10. ""

11. ""

[tap]

1. "G84/G74 - Tap"

3. ""

7. ""

8. ""

9. ""

10. ""

11. ""

[bore1]

1. "G85/G89 - Bore (feed out)"

3. "Dwell - G89"

7. ""

8. ""

9. ""

10. ""

11. ""

[bore2]

1. "G86 - Bore (stop, rapid out)"

7. ""

8. ""

9. ""

10. ""

11. ""

[misc1]

1. "G76 - Fine Bore (shift)"

7. ""

8. ""

9. ""

10. ""

[misc2]

1. "Misc. #2 Drill"

[drill cycle 9]

1. "Subprogram Call"

3. ""

7. "Subprogram Number"

8. ""

9. ""

10. ""

11. ""

[simple drill custom parameters]

1. "Custom Drill Parameters 1"

[peck drill custom parameters]

1. "Custom Drill Parameters 2"

[chip break drill custom parameters]

1. "Custom Drill Parameters 3"

[tap custom parameters]

1. "Custom Drill Parameters 4"

[bore1 custom parameters]

1. "Custom Drill Parameters 5"

[bore2 custom parameters]

1. "Custom Drill Parameters 6"

[misc1 custom parameters]

1. "Custom Drill Parameters 7"

[misc2 custom parameters]

1. "Custom Drill Parameters 8"

[drill cycle 9 custom parameters]

1. "Custom Drill Parameters 9"

[drill cycle 10 custom parameters]

1. "Custom Drill Parameters 10"

[drill cycle 11 custom parameters]

1. "Custom Drill Parameters 11"

[drill cycle 12 custom parameters]

1. "Custom Drill Parameters 12"

[drill cycle 13 custom parameters]

1. "Custom Drill Parameters 13"

[drill cycle 14 custom parameters]

1. "Custom Drill Parameters 14"

[drill cycle 15 custom parameters]

1. "Custom Drill Parameters 15"

[drill cycle 16 custom parameters]

1. "Custom Drill Parameters 16"

[drill cycle 17 custom parameters]

1. "Custom Drill Parameters 17"

[drill cycle 18 custom parameters]

1. "Custom Drill Parameters 18"

[drill cycle 19 custom parameters]

1. "Custom Drill Parameters 19"

[drill cycle 20 custom parameters]

1. "Custom Drill Parameters 20"

[drill cycle descriptions]

1. "G81/G82 - Drill/Counterbore"

2. "G83 - Peck Drill"

3. "G73 - Chip Break"

4. "G84/G74 - Tap"

5. "G85/G89 - Bore (feed out)"

6. "G86 - Bore (stop, rapid out)"

7. "G76 - Fine Bore (shift)"

9. "Subprogram Call"

[canned text]

1. "Stop - M00"

2. "Op Stop - M01"

3. "Bld on"

4. "Bld off"

5. "Dwell - G04 P1"

6. ""

7. ""

8. ""

9. ""

10. ""

[CTRL_TEXT_END]

To set a default for any of the values, just put a double forward slash /> and the value you want as the default.

 

Take a look at the entry for MI #1 in the above code.

 

1. ""//2

 

Even though there is no default text set, the default value is set to '2'.

 

HTH,

Link to comment
Share on other sites
jeff85 Newbie

jeff85

Posted
  • Author
Posted

yea.. the default value for my post is 2 as well.

Its just I have to change the mi1 value for the first operation only to get the correct NC. If I change the 2nd or other operation it will not give me the correct NC.

Anyway, thanks for the help I think I have to manually change it for every job.

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Hi Jeff,

 

I forgot one thing. The Control Definition can now override the default settings in the post.

 

Go to Settings | Machine Definition manager | Click on the 'Edit control defintion' button

 

In the Control definition dialog box, click on "Misc. Int/Real Values" node in the tree. Here you can set the default values for the first operation. Don't get discouraged yet. There is a way to set it so that #2 is set for the default value for the first operation...

 

HTH,

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...