touch off vs tool touch off ?
03 Apr 2016 01:24 #72600
by gizmo6023
touch off vs tool touch off ? was created by gizmo6023
Finally got to try to cut something on the mill today and discovered that setting up the stock does not work as I expected it to.
Using touch off did not move the tool path as I thought it would nor did tool touch off.
What steps do you use to align the stock / tool path to start a job?
I am using Fusion360 for design and cam and end up with the tool path out of machine limits on all three axis on importing the file, machine zero and Fusion zero do not match.
Any tips would be appreciated.
Dave
Using touch off did not move the tool path as I thought it would nor did tool touch off.
What steps do you use to align the stock / tool path to start a job?
I am using Fusion360 for design and cam and end up with the tool path out of machine limits on all three axis on importing the file, machine zero and Fusion zero do not match.
Any tips would be appreciated.
Dave
Please Log in or Create an account to join the conversation.
- kornphlake79
- Offline
- Senior Member
-
Less
More
- Posts: 55
- Thank you received: 10
03 Apr 2016 01:53 - 03 Apr 2016 01:57 #72603
by kornphlake79
Replied by kornphlake79 on topic touch off vs tool touch off ?
You need to be somewhat thoughtful about where you place the origin in fusion 360, it really needs to be on a corner of the part, or somewhere within the part, like the center of the part, or the center of a locating hole. If you have the origin set somewhere off in space, perhaps an assembly origin point, you'll have a hard time locating your toolpath in the machine work envelope.
Assuming your origin is set correctly I normally start up my machine, press the home all button then once the machine is homed I jog each of the axis to the part origin and press the touch off button, the radio button for each axis has to be selected individually and each axis has to be touched off, there isn't a "touch off all" button. Conveniently the radio button automatically moves to which ever axis was last jogged so you don't really have to think about changing that button once you develop a routine.
Assuming your origin is set correctly I normally start up my machine, press the home all button then once the machine is homed I jog each of the axis to the part origin and press the touch off button, the radio button for each axis has to be selected individually and each axis has to be touched off, there isn't a "touch off all" button. Conveniently the radio button automatically moves to which ever axis was last jogged so you don't really have to think about changing that button once you develop a routine.
Last edit: 03 Apr 2016 01:57 by kornphlake79.
Please Log in or Create an account to join the conversation.
03 Apr 2016 11:13 #72612
by BigJohnT
Replied by BigJohnT on topic touch off vs tool touch off ?
I don't know anything about fusion but touch off sets the material location relative to the machine origin. Tool touch off sets the tool table.
gnipsel.com/linuxcnc/g-code/gen05.html
linuxcnc.org/docs/2.7/html/gcode/coordinates.html
linuxcnc.org/docs/2.7/html/gcode/tool-compensation.html
JT
gnipsel.com/linuxcnc/g-code/gen05.html
linuxcnc.org/docs/2.7/html/gcode/coordinates.html
linuxcnc.org/docs/2.7/html/gcode/tool-compensation.html
JT
Please Log in or Create an account to join the conversation.
03 Apr 2016 15:01 #72629
by gizmo6023
Thanks for the links, I read all three and book marked them so they can be referenced as needed in the future.
Since my machine uses an R8 collet I will need to do both touch offs for Z on each tool change?
I see no information for X & Y touch off and what I am getting is not making much sense. I was expecting to set the part X0 Y0 but was getting something quite different, well over 1 inch different than expected.
I will have to adjust where my part zeros are in Fusion as LCNC is placing the part 13 inches above the table and hanging over the left front corner by half the part dimension. I am drawing the part left aft corner on 0,0,0 which should match my machine X0Y0 with no off sets in play.
Dave
Replied by gizmo6023 on topic touch off vs tool touch off ?
touch off sets the material location relative to the machine origin. Tool touch off sets the tool table.
JT
Thanks for the links, I read all three and book marked them so they can be referenced as needed in the future.
Since my machine uses an R8 collet I will need to do both touch offs for Z on each tool change?
I see no information for X & Y touch off and what I am getting is not making much sense. I was expecting to set the part X0 Y0 but was getting something quite different, well over 1 inch different than expected.
I will have to adjust where my part zeros are in Fusion as LCNC is placing the part 13 inches above the table and hanging over the left front corner by half the part dimension. I am drawing the part left aft corner on 0,0,0 which should match my machine X0Y0 with no off sets in play.
Dave
Please Log in or Create an account to join the conversation.
- kornphlake79
- Offline
- Senior Member
-
Less
More
- Posts: 55
- Thank you received: 10
03 Apr 2016 18:34 - 03 Apr 2016 22:39 #72639
by kornphlake79
Replied by kornphlake79 on topic touch off vs tool touch off ?
The part zero in fusion 360 is your G54 zero in LinuxCNC. You have to jog your machine to the part zero (use an edge finder, indicator, etc) then set the G54 offset using the touch off button in Axis. When you press the touch off button make sure the dialog that appears is setting the G54 (or whatever work offset you've programmed in Fusion 360) and the offset value needs to be accurate, for example if you're using an edge finder the offset should be 0.100 inches, either plus or minus depending on where you're touching off, or if you're sweeping a hole with a test indicator the offset should be 0.000.
Last edit: 03 Apr 2016 22:39 by kornphlake79.
Please Log in or Create an account to join the conversation.
03 Apr 2016 20:14 #72648
by BigJohnT
For R8 and similar you just touch off the Z in the G54 coordinate system and ignore the tool touch touch off. I set my X0 to the left side of the part and Y0 the rear of the part. Once you use the edge finder to locate the front edge of the rear jaw on your vise and set that to Y0 your all set on Y. Next chuck up a pin, I use a 1/2" dowel, jog the X axis to just touch the left side of the material and touch off X to -0.250 and now you have the X0 set.
JT
Replied by BigJohnT on topic touch off vs tool touch off ?
Since my machine uses an R8 collet I will need to do both touch offs for Z on each tool change?
I see no information for X & Y touch off and what I am getting is not making much sense. I was expecting to set the part X0 Y0 but was getting something quite different, well over 1 inch different than expected.
I will have to adjust where my part zeros are in Fusion as LCNC is placing the part 13 inches above the table and hanging over the left front corner by half the part dimension. I am drawing the part left aft corner on 0,0,0 which should match my machine X0Y0 with no off sets in play.
Dave
For R8 and similar you just touch off the Z in the G54 coordinate system and ignore the tool touch touch off. I set my X0 to the left side of the part and Y0 the rear of the part. Once you use the edge finder to locate the front edge of the rear jaw on your vise and set that to Y0 your all set on Y. Next chuck up a pin, I use a 1/2" dowel, jog the X axis to just touch the left side of the material and touch off X to -0.250 and now you have the X0 set.
JT
Please Log in or Create an account to join the conversation.
04 Apr 2016 12:39 - 04 Apr 2016 12:42 #72707
by andypugh
If you are using an R8 collet then I would suggest post-processing each tool operation separately into different G-code files.
Load the tool, touch-off the tool-length, load the relevant file and run it. The change tools and run the next file.
You will find that this is more flexible (especially if things go wrong). You may find that in batch-production is it better to run the first op on each part, then the second op on each part, and so on. This does depend on accurate work-fixturing.
This isn't necessarily wrong...
In the CAM part of Fusion you need to set the machining origin in the "setup" section. You can choose the XYZ orientation and pick a part feature or the stock box as origins. By default it picks the part orgin, but that is very unlikely to be the machining origin.
It is very hard to change to part-origin in the part model inside Fusion. Don't bother trying. (It will be the origin point in the first sketch, so you need to redefine the starting sketch)
You then need to jog the CNC machine to the corresponding point on the work / stock and touch of that as the origin.
Replied by andypugh on topic touch off vs tool touch off ?
Since my machine uses an R8 collet I will need to do both touch offs for Z on each tool change?
If you are using an R8 collet then I would suggest post-processing each tool operation separately into different G-code files.
Load the tool, touch-off the tool-length, load the relevant file and run it. The change tools and run the next file.
You will find that this is more flexible (especially if things go wrong). You may find that in batch-production is it better to run the first op on each part, then the second op on each part, and so on. This does depend on accurate work-fixturing.
Check your tool table, it is possible that you have accidentally put X and Y offsets in the tool table.I see no information for X & Y touch off and what I am getting is not making much sense. I was expecting to set the part X0 Y0 but was getting something quite different, well over 1 inch different than expected.
I will have to adjust where my part zeros are in Fusion as LCNC is placing the part 13 inches above the table and hanging over the left front corner by half the part dimension.
This isn't necessarily wrong...
In the CAM part of Fusion you need to set the machining origin in the "setup" section. You can choose the XYZ orientation and pick a part feature or the stock box as origins. By default it picks the part orgin, but that is very unlikely to be the machining origin.
It is very hard to change to part-origin in the part model inside Fusion. Don't bother trying. (It will be the origin point in the first sketch, so you need to redefine the starting sketch)
You then need to jog the CNC machine to the corresponding point on the work / stock and touch of that as the origin.
Last edit: 04 Apr 2016 12:42 by andypugh.
Please Log in or Create an account to join the conversation.
06 Apr 2016 00:38 #72819
by gizmo6023
There may be a misunderstanding on my part on the value to assign to part origin ( assuming it is in the proper place on the part)
is this supposed to be the value displayed on the DRO for the axis being touched off or zero?
Replied by gizmo6023 on topic touch off vs tool touch off ?
If you are using an R8 collet then I would suggest post-processing each tool operation separately into different G-code files.
Load the tool, touch-off the tool-length, load the relevant file and run it. The change tools and run the next file.
You will find that this is more flexible (especially if things go wrong). You may find that in batch-production is it better to run the first op on each part, then the second op on each part, and so on. This does depend on accurate work-fixturing.
Makes perfect sense.
Check your tool table, it is possible that you have accidentally put X and Y offsets in the tool table.I will have to adjust where my part zeros are in Fusion as LCNC is placing the part 13 inches above the table and hanging over the left front corner by half the part dimension.
Tool table was fine but my part origin was in the wrong place.
This isn't necessarily wrong...
In the CAM part of Fusion you need to set the machining origin in the "setup" section. You can choose the XYZ orientation and pick a part feature or the stock box as origins. By default it picks the part orgin, but that is very unlikely to be the machining origin.
It is very hard to change to part-origin in the part model inside Fusion. Don't bother trying. (It will be the origin point in the first sketch, so you need to redefine the starting sketch)
You then need to jog the CNC machine to the corresponding point on the work / stock and touch of that as the origin.
There may be a misunderstanding on my part on the value to assign to part origin ( assuming it is in the proper place on the part)
is this supposed to be the value displayed on the DRO for the axis being touched off or zero?
Please Log in or Create an account to join the conversation.
06 Apr 2016 09:22 #72829
by andypugh
No.
Imagine that the G-code origin in Fusion is set to the left front top corner of the stock.
You can jog your tool down to touch the top of the stock, then touch of the Z to zero.
Then do the same with X and Y to the left and front sides.
Now, when the middle of the end of the tool is at the G-code origin defined in Fusion the DRO will read 0,0,0
In practice you would not normally do it this way. You would use a wiggler or a probe.
If your probe has a 5mm ball on the end you would probe the left side of the stock and touch-off the X-axis to -2.5mm
To set Z height it can be convenient to use a dowel. I use a broken carbide end-mill but I can see a strong argument for using something like brass that can't damage the cutter. Don't jog down to the dowel, jog slowly up until the dowel just slips under the tool.
Then touch-off the coordinate system to the dowel diamter (8mm in my case).
What you are trying to achieve is a DRO reading of 0,0,0 when the tool tip in in the same place as the origin triad in Fusion.
Touch-off is about telling the system where the tool tip _actually_is_ in the CAM coordinate system at the time that you do it.
Replied by andypugh on topic touch off vs tool touch off ?
There may be a misunderstanding on my part on the value to assign to part origin ( assuming it is in the proper place on the part)
is this supposed to be the value displayed on the DRO for the axis being touched off or zero?
No.
Imagine that the G-code origin in Fusion is set to the left front top corner of the stock.
You can jog your tool down to touch the top of the stock, then touch of the Z to zero.
Then do the same with X and Y to the left and front sides.
Now, when the middle of the end of the tool is at the G-code origin defined in Fusion the DRO will read 0,0,0
In practice you would not normally do it this way. You would use a wiggler or a probe.
If your probe has a 5mm ball on the end you would probe the left side of the stock and touch-off the X-axis to -2.5mm
To set Z height it can be convenient to use a dowel. I use a broken carbide end-mill but I can see a strong argument for using something like brass that can't damage the cutter. Don't jog down to the dowel, jog slowly up until the dowel just slips under the tool.
Then touch-off the coordinate system to the dowel diamter (8mm in my case).
What you are trying to achieve is a DRO reading of 0,0,0 when the tool tip in in the same place as the origin triad in Fusion.
Touch-off is about telling the system where the tool tip _actually_is_ in the CAM coordinate system at the time that you do it.
The following user(s) said Thank You: gizmo6023
Please Log in or Create an account to join the conversation.
06 Apr 2016 12:09 #72842
by gizmo6023
Replied by gizmo6023 on topic touch off vs tool touch off ?
Thank you.
I guess part of what is making this difficult to visualize is only my tool path is displayed in AXIS.
Is there a way to display the part as in the Fusion Cam simulation?
I guess part of what is making this difficult to visualize is only my tool path is displayed in AXIS.
Is there a way to display the part as in the Fusion Cam simulation?
Please Log in or Create an account to join the conversation.
Time to create page: 0.186 seconds