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:

Someone care to explain this one??

crazy^millman

By crazy^millman,
in Industrial Forum

 Share

Recommended Posts

crazy^millman Veteran

crazy^millman

Posted
Posted

This one has really got me scratching my head today. I can post this file and I get 2 different outputs all the time. Sometimes I get X positive outputs like I want and sometimes I get negative X output like I done want and even get a different turret selection altogether.

 

Here is the different programs posted 1 minutes a part from the same file using the same post.

 

code:
$LK88950.MIN%

G14

(LOWER TURRET)

(CUSTOMER - ADD CUSTOMER)

(PROGRAMMER - RON
B)

(DATE - SEP. 18 2007)

(TIME - 6:40 AM)<---- Notice the time

(TOOL - 1 - OD ROUGH RIGHT - 80 DEG. LOWER TURRET - OFFSET - 0 - INSERT - CNMG-432 - HOLDER - DCGNR-164D)

(TOOL - 1 OFFSET - 1)

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

N100 G0 X20. Z20. N100 P10

N110 T0101

N120 G18 G95

N130 M109

N140 G97 S212 M03

N150 G0 X3.6 Z.143

N160 X3.5 Z.093

N170 G50 S3000

N180 G96 S200 G111

N700 G85 NAT1 D-.2 U.02 W.01 F.01

N710 NAT1 G81

N720 G0 X2.25 Z.093

N730 G1 G42 Z-.4078

N740 G3 X2.3388 Z-.4847 I.0888

N750 G1 X2.4238 Z-.5092

N760 G2 X2.455 Z-.5363 I-.0156 K-.0271

N770 G1 Z-3.0178

N780 G3 X2.4936 Z-3.0407 I.2762 K.2128

N790 G2 X2.51 Z-3.0618 I-.0231 K-.0211

N800 G1 Z-4.1212

N810 G3 X2.7675 Z-4.25 I.1288

N820 G1 X3.1275

N830 G2 X3.22 Z-4.2962 K-.0462

N840 G1 Z-4.505

N850 G40 X3.5

N860 G80

N100 G0 Z.093

N100 G0 X20. Z20. N100 P20

N110 M05

N120 M02

%

 

$LK88950.MIN%

G14

(LOWER TURRET)

(CUSTOMER - ADD CUSTOMER)

(PROGRAMMER - RON
B)

(DATE - SEP. 18 2007)

(TIME - 6:41 AM)<--- Notice the time

(TOOL - 1 - OD ROUGH RIGHT - 80 DEG. LOWER TURRET - OFFSET - 0 - INSERT - CNMG-432 - HOLDER - DCGNR-164D)

G13

(UPPER TURRET)

(TOOL - 1 OFFSET - 1)

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

G0 X-20. Z20. P10

N1 T0101

G18 G95

M109

G97 S212 M03

G0 X-3.6 Z.143

X-3.5 Z.093

G50 S3000

G96 S200 G110

G85 NAT1 D.2 U-.02 W.01 F.01

NAT1 G81

G0 X-2.25 Z.093

G1 G41 Z-.4078

G3 X-2.3388 Z-.4847 I-.0888

G1 X-2.4238 Z-.5092

G2 X-2.455 Z-.5363 I.0156 K-.0271

G1 Z-3.0178

G3 X-2.4936 Z-3.0407 I-.2762 K.2128

G2 X-2.51 Z-3.0618 I.0231 K-.0211

G1 Z-4.1212

G3 X-2.7675 Z-4.25 I-.1288

G1 X-3.1275

G2 X-3.22 Z-4.2962 K-.0462

G1 Z-4.505

G40 X-3.5

G80

G0 Z.093

G0 X-20. Z20. P20

M05

M02

%

Any suggestions for my sanity are greatly welcomed. Since I am ready to throw everything in the Dumpster. Now this is the weird part to get correctly posted code all I have to do is go into the tool and just go all the way to the set-up and draw the tool not changing anything 3 times and it will give me positive results. If I do the same thing again 3 times I get negative results.

 

Anyone got some ideas I am all ears.

Link to comment
Share on other sites
Jim Evans from CNC Software Newbie

Jim Evans from CNC Software

Posted
Posted

Ron,

 

Not sure what you are using in your post, but start looking at some logic that may modify the sign of X. Dia_mult, scase_ strings, etc.

 

Depending on if you are reading parameters or not, maybe something going on with creation of the OPS file.

 

Another thought is if you have logic where you are checking the equality of values, there may some small difference in the decimal precision and in one case it reads true and then the other false.

 

I'll be glad to give it a try here if you need help.

 

Jim

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
  • Author
Posted

Well just happened again new file same family of parts. Now here is the fix. I just need to edit the tool not changing anything. Go to the set-up and it will now make the operation dirty even though nothing is changed. Now you repost and the X moves now post out as X positive like they are suppose to.

 

Here is the same NC doing the above method:

code:
 G13

(UPPER TURRET)

(TOOL - 5 OFFSET - 5)

(VHR 211 10 4 - VIPV .0938 .04675 INSERT - VIPV .09375 .04375)

G0 X-20. Z20. P150

N5 T0505

G18 G95

G97 S516 M03

G0 X-2.5915 Z-2.6439

G50 S2500

G96 S350 G110

G1 X-2.32 F.004

G0 X-2.5915

Z-2.5946

G1 X-2.32

G0 X-2.5915

Z-2.6932

G1 X-2.32

G0 X-2.5915

Z-2.5453

G1 X-2.32

G0 X-2.5915

Z-2.7425

G1 X-2.32

G0 X-2.5915

Z-2.496

G1 X-2.32

G0 X-2.5915

Z-2.7918

G1 X-2.32

G0 X-2.5915

Z-2.4467

G1 X-2.32

G0 X-2.5915

Z-2.8411

G1 X-2.3207

G0 X-2.5915

Z-2.3974

G1 X-2.32

G0 X-2.5915

Z-2.8903

G1 X-2.333

G0 X-2.5915

Z-2.3481

G1 X-2.32

G0 X-2.5915

Z-2.9396

G1 X-2.361

G2 X-2.333 Z-2.8904 I-.3076 K.1142

G0 X-2.5915 Z-2.8903

Z-2.2988

G1 X-2.3226

G0 X-2.5915

Z-2.9889

G1 X-2.4073

G2 X-2.361 Z-2.9396 I-.2845 K.1635

G0 X-2.5915

Z-2.2495

G1 X-2.4023

G3 X-2.3226 Z-2.2988 I-.027 K-.0626

G0 X-2.5915

Z-3.0382

G1 X-2.4767

G2 X-2.4073 Z-2.989 I-.2498 K.2128

G0 X-2.5915 Z-2.9889

Z-2.1742

X-2.5398

G1 X-2.3984 Z-2.2449

G3 X-2.31 Z-2.3121 I-.029 K-.0672

G1 Z-2.6614

G0 X-2.6105

Z-3.1122

G1 X-2.4691 Z-3.0415

G2 X-2.31 Z-2.8255 I-.2536 K.216

G1 Z-2.6035

G0 X-2.5398

G0 X-20. Z20. P160

M01

Now like it suppose to be:

code:
M01

(TOOL - 5 OFFSET - 5)

(VHR 211 10 4 - VIPV .0938 .04675 INSERT - VIPV .09375 .04375)

G0 X20. Z20. P150

N5 T0505

G18 G95

G97 S516 M03

G0 X2.5915 Z-2.6439

G50 S2500

G96 S350 G111

G1 X2.32 F.004

G0 X2.5915

Z-2.5946

G1 X2.32

G0 X2.5915

Z-2.6932

G1 X2.32

G0 X2.5915

Z-2.5453

G1 X2.32

G0 X2.5915

Z-2.7425

G1 X2.32

G0 X2.5915

Z-2.496

G1 X2.32

G0 X2.5915

Z-2.7918

G1 X2.32

G0 X2.5915

Z-2.4467

G1 X2.32

G0 X2.5915

Z-2.8411

G1 X2.3207

G0 X2.5915

Z-2.3974

G1 X2.32

G0 X2.5915

Z-2.8903

G1 X2.333

G0 X2.5915

Z-2.3481

G1 X2.32

G0 X2.5915

Z-2.9396

G1 X2.361

G2 X2.333 Z-2.8904 I.3076 K.1142

G0 X2.5915 Z-2.8903

Z-2.2988

G1 X2.3226

G0 X2.5915

Z-2.9889

G1 X2.4073

G2 X2.361 Z-2.9396 I.2845 K.1635

G0 X2.5915

Z-2.2495

G1 X2.4023

G3 X2.3226 Z-2.2988 I.027 K-.0626

G0 X2.5915

Z-3.0382

G1 X2.4767

G2 X2.4073 Z-2.989 I.2498 K.2128

G0 X2.5915 Z-2.9889

Z-2.1742

X2.5398

G1 X2.3984 Z-2.2449

G3 X2.31 Z-2.3121 I.029 K-.0672

G1 Z-2.6614

G0 X2.6105

Z-3.1122

G1 X2.4691 Z-3.0415

G2 X2.31 Z-2.8255 I.2536 K.216

G1 Z-2.6035

G0 X2.5398

G0 X20. Z20. P160

M01

I can duplicate this 100 times one 4 different computers with X2MR1SP1 and it is really a pain!!!!!!!!!!!!!!!!!!!!!! Yes QC with the latest release.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
  • Author
Posted

First off I am not crazy as I thought, thanks to Jim Evans and Steve Arteman for pointing out what is going here.

 

When you do an operation you have to check your axis combinations on the operation when you are using the lower Turret. Here is a Picture of what mine defaulted too: TooL_upper_to_start.jpg

 

Here is what it should be:

Tool_lower_changed.jpg

 

So you need to check this everytime you do anything to the operation or to the tool and post the operation. This seems to give the NCI and the information needed to the post a fit if this is not correct.

 

Thanks again to all of those who were helping me with this.

Link to comment
Share on other sites
cappy Newbie

cappy

Posted
Posted

This is exactly what I just spent two days tracking down on an Okuma LR35. Now can someone tell me if I can lock the default to Axis combo left/lower. On the Okumas the G13 (upper turret) & G14 (lower turret) designate the direction of G2's and G3's. In other words a G2 posted out will read the same for both turrets. Depending on the G13 or G14 with determine the direction of arc.

 

Can someone please reccommend a good starting post for an Okuma LR35 OSP 5020-L control that suppports wait codes P10, P20, also live tooling for K values, I values.

 

Thanks in advance,

Greg.

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...