Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

mazak generic milling

6 REPLIES 6
Reply
Message 1 of 7
tillettslawncare
175 Views, 6 Replies

mazak generic milling

I am having troubles editing the post processor, I need would like to alter/change some things in my post. I need it to add a % at the very top of the program before the O# (program number) and after the m30 (program end) Also I would like to move my G49 line to my G30 G91 Z 0. Y 0. so it is cancelled in a move. Lastly I need to take out all my heighth and diameter compensation, I am using my mazatroll tool data so I do not need to use H and D codes. I am currently editing my post (code) in notepad to get the results but would like to have the post spit out what i need. Thank you in advance . 

Reid  

6 REPLIES 6
Message 2 of 7

Give this a try. I've removed the D and H calls, as well as a "%" at the beginning and end. I've not yet touched the location of the G49, that will have to wait until I have some time later or someone else comes along and offers some time.

 

TEST CAREFULLY!


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 7

Thank you for the help I have figured out how to manipulate all but the tool change should look like this T001T01M6   T001 tool in spindle T01 next tool to machine. 
Thanks in advance, Reid 

Message 4 of 7

Does it not run okay the way it is, or is this a matter of wanting it to "look" a certain way?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 7

It’s the way my Mazak calls up tools I believe it has to be that way when using mazatrol tool data. I could be wrong though. 

Message 6 of 7

Nvm, it works with the tool call that way thanks so much for the help! Now I can post with no editing. 
reid 

Message 7 of 7

Hi @seth.madore,

 

One thing to be aware. You need to have a Z axis approach after a G53 Z move and before G5 P2 or you will crash the machine.

 

 

T12 T27 M6 ( T12: CAB_O25HF_Z3 )
S3000 M3
G90 G94 G17
G55
M132 (AR PELO CENTRO)
G0 X45.937 Y-56.171
Z27. <- FIRST Z MOVE BEFORE HIGH-SPEED. LENGTH COMPENSATION ACTIVE
G61.1
G5 P2 <- HIGH-SPEED MODE
G0 Z5.
G1 Z1.4 F7000.
X-45.937
X-56.904
G2 Y-44.961 I0. J5.605
T12 T27 M6 ( T12: CAB_O25HF_Z3 )
S3000 M3
G90 G94 G17
G55
M132 (AR PELO CENTRO)
G0 X45.937 Y-56.171
G61.1
G5 P2 <- HIGH-SPEED MODE
Z27. <- FIRST Z MOVEMENT AFTER HIGH-SPEED ON. NO LENGTH COMPENSATION. WILL CRASH
G0 Z5.
G1 Z1.4 F7000.
X-45.937
X-56.904
G2 Y-44.961 I0. J5.605

 

possamaicadcam_0-1713139551407.png

Regarding the tool call, I answered my own post (another one) through the weekend.

It works fine with the stock post:

T01 M6

T02

The benefit of using T01 T02 M6 is when editing a program we have a function called Quick EIA:

possamaicadcam_1-1713141319271.png

Where I put an arrow, you can move quickly between tool calls inside the program by simply pressing on the list.

But you need to have the current and next tool called on the same line, or it will create a call for the current tool and another one for the next tool.  

 

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report