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: 

Toolpath exceeds the maximum ranges

4 REPLIES 4
SOLVED
Reply
Message 1 of 5
khang.nguyenADB6H
130 Views, 4 Replies

Toolpath exceeds the maximum ranges

Hello,

I was able to generate a tool path with a disc mill however when I used post processor "Doosan Mill/Turn with Fanuc 0i/31i control" to generate NC code it showed error (Toolpath exceeds the maximum ranges for operation "2D Contour3")

Here is what the toolpath looks like

khangnguyenADB6H_0-1701615252282.png

 

 

Here is the error log

Information: Configuration: Doosan Mill/Turn with Fanuc 0i/31i control
Information: Vendor: Doosan
Information: Posting intermediate data to 'C:\Users\KHOI\AppData\Local\Fusion 360 CAM\nc\4333.nc'
Error: Failed to post process. See below for details.
...
Code page changed to '1252  (ANSI - Latin I)'
Start time: Sunday, December 3, 2023 2:48:40 PM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.5991.0
Configuration path: C:/Users/KHOI/AppData/Roaming/Autodesk/Fusion 360 CAM/Posts/doosan mill-turn fanuc 3.cps
Include paths: C:/Users/KHOI/AppData/Roaming/Autodesk/Fusion 360 CAM/Posts
Configuration modification date: Sunday, October 22, 2023 10:48:42 AM
Output path: C:\Users\KHOI\AppData\Local\Fusion 360 CAM\nc\4333.nc
Checksum of intermediate NC data: d93a0e681b21bf8f18d4d376e83345f7
Checksum of configuration: 5123ced806b38553e21a1f574090e235
Legal: Copyright (C) 2012-2023 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.17244
...

###############################################################################
Error: Toolpath exceeds the maximum ranges for operation "2D Contour3".
Error at line: 2639
Error in operation: '2D Contour3'
Failed while processing onSection() for record 483.
###############################################################################

Error: Failed to invoke function 'onSection'.
Error: Failed to invoke 'onSection' in the post configuration.
Error: Failed to execute configuration.
Stop time: Sunday, December 3, 2023 2:48:40 PM
Post processing failed.

 

Thank you

Labels (1)
4 REPLIES 4
Message 2 of 5

Hi

 

This is because the toolpath is larger than the Y-axis travel for your machine as set in the post processor.

Most machines have only +-50mm travel, the toolpath is 116mm

alaasW8M6T_0-1701623457684.png

 

What is the Y axis travel for your particular machine, you didn't mention which one you have?

Message 3 of 5

Hi a.laasW8M6T,

 

I'm currently using PUMA 2600 SYBII from DN Solutions, this is what has been specified inside of its specification for Y-axis travel. Could you please show me how to adjust Y-axis travel inside the post processor. Thank you.

khangnguyenADB6H_0-1701652642677.png

 

 

 

Message 4 of 5

You can adjust it in the post processor, but your toolpath will still exceed the travel limits as the end of the slot is 54.224mm from centerline and you only have 52.5mm travel

alaasW8M6T_0-1701664961447.png

That is with making the lead in radius zero too.

 

The part is just too big to be machined with a tool like that in the Y axis.

 

You would need to slot it with a tiny 1.5mm endmill using the X axis travel instead

 

 

If you do wish to edit the post you can search for lines 933 and 934 and change the values there for the Puma model type

alaasW8M6T_1-1701665180126.png

 

Message 5 of 5

Thanks. I successfully adjusted the post processor and created NC code.

khangnguyenADB6H_0-1701695110351.png

 

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

Post to forums  

Autodesk Design & Make Report