GCode file doesn't do what I expect
07 Aug 2018 06:51 - 07 Aug 2018 06:52 #115731
by CNCKoala
GCode file doesn't do what I expect was created by CNCKoala
Hi All, I need some help before I go mad
and broke ... Also I hope that this is in the right discussion thread - happy to move it elsewhere if so advised ![:) :)](/media/kunena/emoticons/smile.png)
I have managed to set up LinuxCNC and configure it to run my CNC mill. Using the keyboard to jog all the axis' works fine and without any issues. The problem I am having is when it comes to run a file.
Here are the steps I am taking:
At this point I am expecting the Z axis to lift about 5mm move to the starting point on the job and get stuck in. Instead I am usually getting an error message that says that one or more of the axis exceed the machine limits, and when I choose, Continue Anyway, it just plunges the tool straight down through the material.
![:angry: :angry:](/media/kunena/emoticons/angry.png)
So far I am on my 4th end mill bit, and have decided that enough is enough and the challenge is outside of my skill set to resolve.
Not sure what files I should attach to help out so if anyone thinks that they might know what is causing the issues, let me know what you need to help confirm and I will provide
Thanks again in advance
![:side: :side:](/media/kunena/emoticons/sideways.png)
![:S :S](/media/kunena/emoticons/dizzy.png)
![:) :)](/media/kunena/emoticons/smile.png)
I have managed to set up LinuxCNC and configure it to run my CNC mill. Using the keyboard to jog all the axis' works fine and without any issues. The problem I am having is when it comes to run a file.
Here are the steps I am taking:
- Jog the tool to the front left corner of the mill, just touching the spoil board
- Set all axis as home at this point - however I have noticed that the values for X, Y and Z are not changed to '0' when I do this
- Jog the machine to the required starting point on the material and 'Touch Off' X and Y axis
- Check that the machine has enough range of movement for the job
- Move the Z axis to the top of the material and 'Touch Off' this axis
- Run the job
At this point I am expecting the Z axis to lift about 5mm move to the starting point on the job and get stuck in. Instead I am usually getting an error message that says that one or more of the axis exceed the machine limits, and when I choose, Continue Anyway, it just plunges the tool straight down through the material.
![:( :(](/media/kunena/emoticons/sad.png)
![:angry: :angry:](/media/kunena/emoticons/angry.png)
![:( :(](/media/kunena/emoticons/sad.png)
![:angry: :angry:](/media/kunena/emoticons/angry.png)
So far I am on my 4th end mill bit, and have decided that enough is enough and the challenge is outside of my skill set to resolve.
Not sure what files I should attach to help out so if anyone thinks that they might know what is causing the issues, let me know what you need to help confirm and I will provide
Thanks again in advance
Last edit: 07 Aug 2018 06:52 by CNCKoala.
Please Log in or Create an account to join the conversation.
- tommylight
-
- Away
- Moderator
-
Less
More
- Posts: 18524
- Thank you received: 6191
07 Aug 2018 07:26 #115732
by tommylight
Replied by tommylight on topic GCode file doesn't do what I expect
Hal and ini file should help as it seems you have some settings wrong in the ini file.
Also more informations about the machine is always helpful.
2001 !!!
Also more informations about the machine is always helpful.
2001 !!!
Please Log in or Create an account to join the conversation.
07 Aug 2018 07:49 #115733
by CNCKoala
Replied by CNCKoala on topic GCode file doesn't do what I expect
Thanks tommylight, hopefully these are what you need. I have also attached the test file I was trying out.
The router is a 6040 I purchased off 'EvilBay' some time ago but have recently moved from MACH3 and having to set it all up again![:) :)](/media/kunena/emoticons/smile.png)
Work ares dimensions are:
X = 280mm
Y = 390mm
Z= 55mm
Touch off points were at X60; Y70, Z20
Cheers
The router is a 6040 I purchased off 'EvilBay' some time ago but have recently moved from MACH3 and having to set it all up again
![:) :)](/media/kunena/emoticons/smile.png)
Work ares dimensions are:
X = 280mm
Y = 390mm
Z= 55mm
Touch off points were at X60; Y70, Z20
Cheers
Please Log in or Create an account to join the conversation.
- tommylight
-
- Away
- Moderator
-
Less
More
- Posts: 18524
- Thank you received: 6191
07 Aug 2018 07:56 #115734
by tommylight
Replied by tommylight on topic GCode file doesn't do what I expect
You need to set the Z axis ( axis 2 ) to -55 to be able to use it.
Also whatever you use for CAM to output the gcode, set it so it has the surface of the part as 0 for the Z axis.
As you have it set you have cuts in the + and in the minus side of the Z axis, and is a mess.
Other settings look OK.
Also whatever you use for CAM to output the gcode, set it so it has the surface of the part as 0 for the Z axis.
As you have it set you have cuts in the + and in the minus side of the Z axis, and is a mess.
Other settings look OK.
Please Log in or Create an account to join the conversation.
07 Aug 2018 08:54 #115735
by CNCKoala
Replied by CNCKoala on topic GCode file doesn't do what I expect
Thanks tommylight for this, will adjust the config file in the morning so Z axis is from -55 to 0 rather than 0 to 55, and then give it another go
I am learning to use Fusion360 as my CAD / CAM software, because my previous choices (Solidworks and Vectric Aspire) are now no longer within my budget. I wioll also adjust my test file CAM output to reflect your suggestions
Cheers and thanks again
I am learning to use Fusion360 as my CAD / CAM software, because my previous choices (Solidworks and Vectric Aspire) are now no longer within my budget. I wioll also adjust my test file CAM output to reflect your suggestions
Cheers and thanks again
Please Log in or Create an account to join the conversation.
14 Aug 2018 15:51 #116054
by andypugh
Replied by andypugh on topic GCode file doesn't do what I expect
Just to elaborate. This is Fusion's fault, not yours.
Fusion starts with
N20 G53 G0 Z0.
Which is a move to Z = 0 in _absolute_ coordinates.
And in your config that is the bottom, not the top, of travel.
0 at the bottom and 55 at the top is perfectly sensible and logical, but Fusion assumes that 0 is at the top and that it is requesting a retract, not a plunge through the table.
So, as mentioned, the fix is to have 0 at the top and -55 at the bottom.
I hate this assumption by Fusion360 CAM (though actually it is an assumption by the post-processor, really)
Fusion starts with
N20 G53 G0 Z0.
Which is a move to Z = 0 in _absolute_ coordinates.
And in your config that is the bottom, not the top, of travel.
0 at the bottom and 55 at the top is perfectly sensible and logical, but Fusion assumes that 0 is at the top and that it is requesting a retract, not a plunge through the table.
So, as mentioned, the fix is to have 0 at the top and -55 at the bottom.
I hate this assumption by Fusion360 CAM (though actually it is an assumption by the post-processor, really)
Please Log in or Create an account to join the conversation.
14 Aug 2018 22:57 #116066
by CNCKoala
Replied by CNCKoala on topic GCode file doesn't do what I expect
Thank you andypugh to pick up that while I was incorrect I was not that wrong.
There is so much to learn as you move from one environment, piece of software, to another.
I am only just figuring out some of the basics and asking questions on forums is a learning process as well for me.
The information on the internet can be great but also very confusing at times for the newcomer as a level a prior knowledge is often expected from those that make the information available.
Cheers
There is so much to learn as you move from one environment, piece of software, to another.
I am only just figuring out some of the basics and asking questions on forums is a learning process as well for me.
The information on the internet can be great but also very confusing at times for the newcomer as a level a prior knowledge is often expected from those that make the information available.
Cheers
Please Log in or Create an account to join the conversation.
15 Aug 2018 00:34 #116067
by andypugh
I wouldn't even go that far. I think that this is incorrect behaviour on the part of Fusion360 and it is probably causing a lot of broken bits and ruined tables.
Replied by andypugh on topic GCode file doesn't do what I expect
Thank you andypugh to pick up that while I was incorrect I was not that wrong.
I wouldn't even go that far. I think that this is incorrect behaviour on the part of Fusion360 and it is probably causing a lot of broken bits and ruined tables.
Please Log in or Create an account to join the conversation.
15 Aug 2018 03:04 - 15 Aug 2018 03:15 #116069
by snoozer77
Replied by snoozer77 on topic GCode file doesn't do what I expect
I have modified the post processor to not do the initial G53 zero move (only because the machine is large and slow). Doing that in your case would allow you to put your Z machine coordinates as either +55 or -55 at the top.
Saying that, on all the mills i have ever used,G53 Z0 is always at the top of travel, going to negative. I guess whoever writes fusion post processors are assuming this.
Saying that, on all the mills i have ever used,G53 Z0 is always at the top of travel, going to negative. I guess whoever writes fusion post processors are assuming this.
Last edit: 15 Aug 2018 03:15 by snoozer77.
Please Log in or Create an account to join the conversation.
15 Aug 2018 03:06 #116070
by snoozer77
Replied by snoozer77 on topic GCode file doesn't do what I expect
Now i think about it though, the machine bed at Z0 does sound logical...
Please Log in or Create an account to join the conversation.
Time to create page: 0.136 seconds