End mill driving through material on first cut
18 Jul 2016 08:58 #77589
by swalts
End mill driving through material on first cut was created by swalts
Hello and thank you for taking the time.
I have attempted to make 6 different objects with Fusion 360 and Linuxcnc. The hardware is sound as Fusion and Linuxcnc seem to play nice while engraving.
My latest attempt at milling aluminum has failed once again. The machine drives the mill straight through the material and then tries to keep going. This has been ongoing for some time now.
I am certain there is something wrong in the way I am setting things up. Would someone or everyone, please show/ explain what is wrong so I can correct my errors.
I can walk you through what i do when attempting to run the g-code. Please correct me where necessary.
I have attempted to make 6 different objects with Fusion 360 and Linuxcnc. The hardware is sound as Fusion and Linuxcnc seem to play nice while engraving.
My latest attempt at milling aluminum has failed once again. The machine drives the mill straight through the material and then tries to keep going. This has been ongoing for some time now.
I am certain there is something wrong in the way I am setting things up. Would someone or everyone, please show/ explain what is wrong so I can correct my errors.
I can walk you through what i do when attempting to run the g-code. Please correct me where necessary.
- load g-code profile.
- Home all axis
- clear all offsets previously set
- center end mill on my target (usually the center)
- run z-axis down to fine tune x,y position on my target.
- once all three axis are set in position, I touch off on all three axis's
- raise z-axis half way to home.
- turn on router
- press "run"
- The machine runs up further and asks for a tool. (installed already)
- click through and watch the crash
- hit emergency stop.
Very Respectfully,
Steve
Please Log in or Create an account to join the conversation.
18 Jul 2016 09:52 #77590
by andypugh
Replied by andypugh on topic End mill driving through material on first cut
Looking at the G-code it appears that my first guess was wrong, you have actually set the CAM origin of the setup to the top of the work.
So, I think that you have missed out a step in your setup:
3a) Load the tool and apply the tool offset (M6 T1 G43)
I think that your problem is that you are starting with no loaded tool and no tool offset, then this line of the G-code:
N60 G43 Z0.6 H1
Is applying tool-offset number 1, which is non-zero.
To be doubly sure you might want to edit your tool table and remove the offsets.
So, I think that you have missed out a step in your setup:
3a) Load the tool and apply the tool offset (M6 T1 G43)
I think that your problem is that you are starting with no loaded tool and no tool offset, then this line of the G-code:
N60 G43 Z0.6 H1
Is applying tool-offset number 1, which is non-zero.
To be doubly sure you might want to edit your tool table and remove the offsets.
The following user(s) said Thank You: swalts
Please Log in or Create an account to join the conversation.
18 Jul 2016 20:28 #77616
by swalts
Replied by swalts on topic End mill driving through material on first cut
Thank you, AndyPugh
I will try this out once i figure out how to load a tool offset. I will return back to post results either positive or negative. I am interested to know if I should load the tool parameters in fusion 360 then figure out how to do in linuxcnc. What is your take on the matter?
Thanks,
-Steve
I will try this out once i figure out how to load a tool offset. I will return back to post results either positive or negative. I am interested to know if I should load the tool parameters in fusion 360 then figure out how to do in linuxcnc. What is your take on the matter?
Thanks,
-Steve
Please Log in or Create an account to join the conversation.
18 Jul 2016 21:43 #77619
by andypugh
Replied by andypugh on topic End mill driving through material on first cut
Fusion assumes that the tool-table is correct. (This is why it does G43).
From your description of the process it sounds like you are not actively using the tool table, so you probably want it all-zeros.
G10 is one way to do this. The tool table editor is another. An arbitrary text editor is a third....
Amongst the ways to edit the tool table are such disparate elements as....
From your description of the process it sounds like you are not actively using the tool table, so you probably want it all-zeros.
G10 is one way to do this. The tool table editor is another. An arbitrary text editor is a third....
Amongst the ways to edit the tool table are such disparate elements as....
Please Log in or Create an account to join the conversation.
19 Jul 2016 09:19 #77630
by swalts
Replied by swalts on topic End mill driving through material on first cut
SUCCESS!!!
I modified the tool library in fusion 360 and allowed tool write for post process. Then I modified tool in tool table so both software matched. The cutting performed very nicely. I consider this topic closed. Thank you all for your time and patience. Now I just have to true up my machine so I can get even cutting.
I modified the tool library in fusion 360 and allowed tool write for post process. Then I modified tool in tool table so both software matched. The cutting performed very nicely. I consider this topic closed. Thank you all for your time and patience. Now I just have to true up my machine so I can get even cutting.
Please Log in or Create an account to join the conversation.
19 Jul 2016 10:46 #77633
by andypugh
I _haven't_ done this, and still get the right results.
I don't actually think that what you have done is the best solution. I suspect that if you now change the length of your tool and change the tool table to suit you might not be able to re-use the same G-code.
Does Your G-code still have Z=0 as the top of the work, or is there now an explicit tool offset in the G-code?
Replied by andypugh on topic End mill driving through material on first cut
I modified the tool library in fusion 360 and allowed tool write for post process. Then I modified tool in tool table so both software matched..
I _haven't_ done this, and still get the right results.
I don't actually think that what you have done is the best solution. I suspect that if you now change the length of your tool and change the tool table to suit you might not be able to re-use the same G-code.
Does Your G-code still have Z=0 as the top of the work, or is there now an explicit tool offset in the G-code?
Please Log in or Create an account to join the conversation.
19 Jul 2016 14:25 - 19 Jul 2016 14:31 #77646
by swalts
Replied by swalts on topic End mill driving through material on first cut
You are probably correct. If you have the time and are willing, would post some sort of laman terms walkthrough. Touching on the subject of tools. As you no doubt have discovered i am very new to milling and have not developed a proper vocabulary yet.
I could use information on setting up the tool table.
Homing and zeroing. Proper procedure from starting controller to end of machining process.
I realize its a tall order, but i am sincere.
On another note, here is the revised g-code
Thank you for your time.
-Steve
I could use information on setting up the tool table.
Homing and zeroing. Proper procedure from starting controller to end of machining process.
I realize its a tall order, but i am sincere.
On another note, here is the revised g-code
Thank you for your time.
-Steve
Last edit: 19 Jul 2016 14:31 by swalts.
Please Log in or Create an account to join the conversation.
20 Jul 2016 21:27 #77737
by andypugh
Replied by andypugh on topic End mill driving through material on first cut
This is what I do. It is just one way of several. It helps to understand the offsets:
linuxcnc.org/docs/2.7/html/gcode/coordinates.html
linuxcnc.org/docs/2.7/html/gcode/tool-compensation.html
I have arbitrarily decided that my touch-probe has a reference length of zero. Every other tool has an offset in the tool-table relative to that tool.
If I touch-off the work top-surface to zero with the probe, and the tool has zero-offsets for the probe tool (99 in my case) then any other tool needs a tool-table entry to allow for how much longer or shorter than the probe it is.
So, I start with the probe, and set the current coordinate system (almost always G54) so that the probe at the top of the work shows zero.
Then I could load a tool, and touch-off that tool to the _Tool_Table_. ie, set a tool-table entry for that tool so that it agrees with the probe about where the top of the work is.
(Actually this is how it works on the lathe, on the Mill I actually have an offline height-measuring jig, and work in a different way)
What works for you might be different again. But you have to be clear on the offect of work offsets and tool offsets, and realise that unless there is a value of zero in the tool-table for the tool you just loaded then G43 will move the working point.
linuxcnc.org/docs/2.7/html/gcode/coordinates.html
linuxcnc.org/docs/2.7/html/gcode/tool-compensation.html
I have arbitrarily decided that my touch-probe has a reference length of zero. Every other tool has an offset in the tool-table relative to that tool.
If I touch-off the work top-surface to zero with the probe, and the tool has zero-offsets for the probe tool (99 in my case) then any other tool needs a tool-table entry to allow for how much longer or shorter than the probe it is.
So, I start with the probe, and set the current coordinate system (almost always G54) so that the probe at the top of the work shows zero.
Then I could load a tool, and touch-off that tool to the _Tool_Table_. ie, set a tool-table entry for that tool so that it agrees with the probe about where the top of the work is.
(Actually this is how it works on the lathe, on the Mill I actually have an offline height-measuring jig, and work in a different way)
What works for you might be different again. But you have to be clear on the offect of work offsets and tool offsets, and realise that unless there is a value of zero in the tool-table for the tool you just loaded then G43 will move the working point.
Please Log in or Create an account to join the conversation.
Time to create page: 0.126 seconds