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:

5 AXIS DRILLING NOT ACCURATE


CARLOS_951
 Share

Recommended Posts

ANY INSIGHT ON WHY MY BASIC POST AND THE FUNCTION 5 AXIS DRILLING DOES NOT POST OUT CORRECT? IM USING GENERIC HAAS VF-TR_SERIES 5X MILL. WRONG X,Y,A, AND B'S. IM PROGRAMMING OFF C/L ROTATION. IM 100% SELF TAUGHT LAST 5 YEARS. 

LET ME KNOW WHAT YOU GUYS THINK I CAN SEND YOU MY FILE. 

Link to comment
Share on other sites
17 hours ago, CARLOS_951 said:

ANY INSIGHT ON WHY MY BASIC POST AND THE FUNCTION 5 AXIS DRILLING DOES NOT POST OUT CORRECT? IM USING GENERIC HAAS VF-TR_SERIES 5X MILL. WRONG X,Y,A, AND B'S. IM PROGRAMMING OFF C/L ROTATION. IM 100% SELF TAUGHT LAST 5 YEARS. 

LET ME KNOW WHAT YOU GUYS THINK I CAN SEND YOU MY FILE. 

I think more people would show up with ideas if they could hear you... CAPS is considered yelling on Internet forums... 

Link to comment
Share on other sites
7 minutes ago, Watcher said:

I think more people would show up with ideas if they could hear you... CAPS is considered yelling on Internet forums... 

Nah :)

He just shared nothing.....his positions off...great, where's the file....my guess is he either doesn't have the WCS/Planes set up right OR he is using an unproven post that is not yet set up for his machine....another possibility is his part is not set up in the correct orientation for his machine.

but all we know to this point is he gets wrong output from his post  

 

Edited by Guest
Link to comment
Share on other sites

Here is my file. 

Quote

Are setup correctly on the has trunion. Is this an older one were you need to figure out were the center of rotation is above the platter? Some wereason between .1 and .16 or so.  So this is always origin? 

C/L of rotation is 2.00" above plater, i have that set up. 

Quote

He just shared nothing.....his positions off...great, where's the file....my guess is he either doesn't have the WCS/Planes set up right OR he is using an unproven post that is not yet set up for his machine....another possibility is his part is not set up in the correct orientation for his machine.

but all we know to this point is he gets wrong output from his post  

It is an unproven post the most generic post that comes with mastercam. Again self taught on this dont know how to edit posts. Part is orientated correctly for the machine otherwise the rest of the program would of been junk. 

 

 

Edited by gcode
ITAR File deleted
Link to comment
Share on other sites

Well, there is NO way your OP2 posted out correct......everything posts to A0 B0 for your milling paths

You need to set ALL of your WCS's to TOP......your planes will stay exactly as you have them set...

 

Here's your numbers as set

(1/4 SPOTDRILL|TOOL - 5|DIA. OFF. - 5|LEN. - 5| DIA. - .25)
M11
M13
T5 M6
G0 G54 G90 X-1.6084 Y.1445 B180. A90. S1500 M3
M10
M12
G43 H5 Z10.
G81 G99 Z8.24 R10. F5.
G80
X-.198 Y6.8125 B178.435 A-34.655
G81 G99 Z9.3 R10. F5.
G80
(SPOT ALL HOLES)
X-.0818 Y.5573 B174.771 A-7.595
G81 G99 Z8.2845 R10. F5.
G80
X-.1824 Y4.363 B177.778 A-23.591
G81 G99 Z7.7553 R10. F5.
G80
M5
G0 G28 G91 Z0.
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
(NO. 41 DRILL|TOOL - 70|DIA. OFF. - 70|LEN. - 70| DIA. - .096)
M11
M13
T70 M6
G0 G54 G90 X.1824 Y-4.363 B-2.222 A23.591 S1500 M3
M10
M12
G43 H70 Z10.
G81 G99 Z7.7553 R10. F5.
G80
X.198 Y-6.8125 B-1.565 A34.655
G81 G99 Z6.682 R10. F5.
G80
X.3222 Y2.1407 B6.375 A-3.769
G81 G99 Z8.2473 R10. F5.
G80
(SPOT ALL HOLES)
X.0818 Y-.5573 B-5.229 A7.595
G81 G99 Z8.2845 R10. F5.
G80
M5
G0 G28 G91 Z0.
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
(.100 REAMER|TOOL - 250|DIA. OFF. - 250|LEN. - 250| DIA. - .1)
M11
M13
T250 M6
G0 G54 G90 X-.3222 Y-2.1407 B186.375 A3.769 S350 M3
M10
M12
G43 H250 Z10.
G85 G99 Z8.05 R10. F3.
G80
X-.198 Y6.8125 B178.435 A-34.655
G85 G99 Z6.682 R10. F3.
G80
(SPOT ALL HOLES)
X-.0818 Y.5573 B174.771 A-7.595
G85 G99 Z8.2845 R10. F3.
G80
X-.1824 Y4.363 B177.778 A-23.591
G85 G99 Z7.7553 R10. F3.
G80
M5
G0 G28 G91 Z0.
M30
%

 

and after setting them all to TOP you can see the differences

(1/4 SPOTDRILL|TOOL - 5|DIA. OFF. - 5|LEN. - 5| DIA. - .25)
M11
M13
T5 M6
G0 G54 G90 X-1.6084 Y.1445 B180. A90. S1500 M3
M10
M12
G43 H5 Z10.
G81 G99 Z8.24 R10. F5.
G80
Z35.3763
X427.2259 Y-109.7232
M11
M13
B91.424 A38.651
M10
M12
G81 G99 Z34.6763 R35.3763 F5.
G80
(SPOT ALL HOLES)
M11
M13
B90.757 A65.726
M10
M12
X427.9569 Y-112.7073
Z-15.9073
G81 G99 Z-17.6229 R-15.9073 F5.
G80
Z14.0097
X427.5044 Y-113.6252
M11
M13
B91.165 A49.718
M10
M12
G81 G99 Z11.765 R14.0097 F5.
G80
M5
G0 G28 G91 Z0.
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
(NO. 41 DRILL|TOOL - 70|DIA. OFF. - 70|LEN. - 70| DIA. - .096)
M11
M13
T70 M6
G0 G54 G90 X427.5044 Y-113.6252 B91.165 A49.718 S1500 M3
M10
M12
G43 H70 Z14.0097
G81 G99 Z11.765 R14.0097 F5.
G80
Z35.3763
X427.2259 Y-109.7232
M11
M13
B91.424 A38.651
M10
M12
G81 G99 Z32.0583 R35.3763 F5.
G80
M11
M13
B90.429 A77.034
M10
M12
X428.2931 Y-107.6043
Z-35.2248
G81 G99 Z-36.9774 R-35.2248 F5.
G80
(SPOT ALL HOLES)
Z-15.9073
X427.9569 Y-112.7073
M11
M13
B90.757 A65.726
M10
M12
G81 G99 Z-17.6229 R-15.9073 F5.
G80
M5
G0 G28 G91 Z0.
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
(.100 REAMER|TOOL - 250|DIA. OFF. - 250|LEN. - 250| DIA. - .1)
M11
M13
T250 M6
G0 G54 G90 X428.2931 Y-107.6043 B90.429 A77.034 S350 M3
M10
M12
G43 H250 Z-35.2248
G85 G99 Z-37.1748 R-35.2248 F3.
G80
Z35.3763
X427.2259 Y-109.7232
M11
M13
B91.424 A38.651
M10
M12
G85 G99 Z32.0583 R35.3763 F3.
G80
(SPOT ALL HOLES)
M11
M13
B90.757 A65.726
M10
M12
X427.9569 Y-112.7073
Z-15.9073
G85 G99 Z-17.6229 R-15.9073 F3.
G80
Z14.0097
X427.5044 Y-113.6252
M11
M13
B91.165 A49.718
M10
M12
G85 G99 Z11.765 R14.0097 F3.
G80
M5
G0 G28 G91 Z0.
M30

Now that's a BIG part of your issue....

The other is there are some wildly large numbers in your plane settings causing some HUGE numbers to be output....I'm not digging into that....but it looks like you need to move your part to the system origin

I suggest you get with your local reseller

Reseller: CAD/CAM Consulting Services INC.
Reseller URL: http://www.cad-cam.com
Contact: Tom Shelar
Phone: 805-375-7676
Email: [email protected]
Edited by Guest
Link to comment
Share on other sites

To your PM, sorry, I help on the forum, it leaves a trail for others to follow if they run into a similar issue.

7 minutes ago, CARLOS_951 said:

Why do you have to set it to system origin? You cant just make your own origin for this? 

As to your question, historically, it has always been the best practice to work off the system origin for any rotary and/or 5 axis work

Link to comment
Share on other sites
On 5/28/2017 at 9:34 AM, JParis said:

...historically, it has always been the best practice to work off the system origin for any rotary and/or 5 axis work

If you're using a Mastercam post. ;) 

When using a 3rd Party post like say CAMplete... makes no difference. :)

Link to comment
Share on other sites
On 5/28/2017 at 9:34 AM, JParis said:

To your PM, sorry, I help on the forum, it leaves a trail for others to follow if they run into a similar issue.

Yep. If one person has a question, chances are, out there someone else has the very same question/issue. 

Link to comment
Share on other sites
37 minutes ago, Foghorn Leghorn said:

If you're using a Mastercam post. ;) 

When using a 3rd Party post like say CAMplete... makes no difference. :)

That's how we do it. I have several parts with origins on the top and bottom.

 

It makes it easy to adjust when you use a different riser or fixture 

  • Like 1
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

  • 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.

Follow us

×
×
  • Create New...