Transforming Rotary Mill in an Okuma

[rrichard]

   Morning,

    Looked but couldn't find info I needed.

   The sample file attached is a simple example of my issues, simple contour on a 4" OD round, then transformed for a total of 4 cuts. MC looks fine, but when I post all 4 locations are at the same angles,

  Thank you for any help

Russell

T.mcx-9

[jeff]

Your Transform page looks identical to mine with the exception of Work Offset Numbering. Mine is set to "Maintain Source Operations".

Try that, but I don't think that is the issue.

 

Also I noticed you have top of stock to Z0 Absolute. Maybe that's causing problems as well.

[rrichard]

Thanks Jeff, I'll see what stock will do?

[ajmer]

you cannot rotate a axis sub toolpath

change to translate in Y

 

ajmer_ihs_T.mcx-9

[rrichard]

Thank you AJ, I see what you did and it works fine, only thing it's still posting all Identical "A moves" ???

I tried with the Okuma post and the HAAS post and all the same moves??

Thanks

Russell

[jlw™]

This is one of my hangups with translate, you could have already made unique paths and been done.  I would only chase translate if I had a lot of features.  With 4, I'd path it the way I want and be done.

jm2c

[Greg Williams]

Seems okay here with an old  MPmaster post

 

O0001
(T)
(FILE  - T.MCX-9)
(PROGRAM   - T.MIN)
(DATE      - 02-APR-17)
(TIME      - 16:27)
 
(285 - 1/4 FLAT ENDMILL          - H285 - D285 - D0.2500" )
 
G00 G17 G20 G40 G80 G90
G00 G16 H0 Z999.
(OPERATION NUMBER - 1)
(WCS NAME - TOP)
(TOOLPLANE NAME - TOP)
IF [VTLCN EQ 285] N1 (SPINDLE TOOL CHECK)
T285 (1/4 FLAT ENDMILL)
M6
N1 (SPINDLE TOOL JUMP)
S2139 M03
G15 H1
M11 (UNLOCK)
G00 G90 X.3827 Y0. A0. M15
G56 H=VTLCN Z2.25
G131 J0 E.001 D0.0005 I0 F20000 (SUPERNURBS ROUGHING)
Z2.2
G01 Z1.8 F6.42
X.5453
A342.053 M16
X-.5453
A17.947 M15
X.5453
A0. M16
X.3827
Z2.
G00 Z2.25
M11 (UNLOCK)
X.3827 Y0. Z2.25 A90. M16
Z2.2
G01 Z1.8
X.5453
X-.5453
X.5453
X.3827
Z2.
G00 Z2.25
M11 (UNLOCK)
X.3827 Y0. Z2.25 A180. M15
Z2.2
G01 Z1.8
X.5453
X-.5453
X.5453
X.3827
Z2.
G00 Z2.25
M11 (UNLOCK)
X.3827 Y0. Z2.25 A270. M15
Z2.2
G01 Z1.8
X.5453
X-.5453
X.5453
X.3827
Z2.
G00 Z2.25
G130 (SUPER NURBS OFF)
M05
G00 G16 H0 Z999.
S300 M03
M12 (TOOL CLEANING AIR BLOW)
G04 P3.0
M09
M05
M11 (UNLOCK)
A0.
M10 (LOCK)
G90
M02
%

 

 

[crazy^millman]

There is a known bug with trying to translate Axis subs. There is a in on the Mastercam web site that talks about how to trick Mastercam into doing it. We had a topic in last few months were someone was having the issue. I sent it to QC and after a lengthy discussion they are looking at a better way to handle these situations. Sorry have not looked at the file, but just an FYI for those looking to transform an Axis sub there is known issues. There is work around, but I tested previously and got A repeating and not going around the part like it should. Greg got good output so it might be the way the newer post are handling things. I will try to remember to look at the file this week, but looks like you are already well on your way. 

[huskermcdoogle]

https://kb.mastercam.com/KnowledgebaseArticle50169.aspx

Here is the knowledge base article.

[rrichard]

Thanks to all for the help.

  huskermcdoogle,  Knowledgebase with the points w/ our post work perfect.

Thank you again Russell 

[jeff]

On 3/30/2017 at 1:10 PM, ajmer said:

you cannot rotate a axis sub toolpath

change to translate in Y

 

ajmer_ihs_T.mcx-9

Interesting, I wonder if that's why I have errors sometimes when translating for my rotary.