Tool change on single project

[keithc]

Not sure if its a capability or not. But I have a small project I want to start off by pocket clearing with a 1/4 end mill using fusion 360 then finishing with a 1/8 end mill. I cant use two processes with the same zero point because I am using top let of my stock as zero. I have the process posted with both bits but universal gcode sees it as one tool and continues on through. the only option I see is making two processes and on my 1/8 pass re zero to the model and start prom there, The only problem with that is accuracy. as we all know manually setting the start point and milling a part doesn't take much to be off. I hope I'm being clear here. And using the return to zero on UGCS is useless. it just does whatever it wants. and it seems I cant figure out a way to start/return/start from home. and yes I have homing switches installed.

[aforww]

Feb 12, 2017 16:01:49 GMT keithc said:

Not sure if its a capability or not. But I have a small project I want to start off by pocket clearing with a 1/4 end mill using fusion 360 then finishing with a 1/8 end mill. I cant use two processes with the same zero point because I am using top let of my stock as zero. I have the process posted with both bits but universal gcode sees it as one tool and continues on through. the only option I see is making two processes and on my 1/8 pass re zero to the model and start prom there, The only problem with that is accuracy. as we all know manually setting the start point and milling a part doesn't take much to be off. I hope I'm being clear here. And using the return to zero on UGCS is useless. it just does whatever it wants. and it seems I cant figure out a way to start/return/start from home. and yes I have homing switches installed.

Well first things first, we need to fix your homing situation.

What are the steps you take when establishing machine home and for setting your work piece home?

[Derek the Admin]

You will have to break it into two different files because Fusion generated G code is probably issuing tool change commands which grbl is just ignoring because the kind of machines grbl (the control firmware) was meant to run will pretty much never have an auto tool changer.

You can use Work Coordinate Systems to pick up the same position over and over again. Jog to where you want the origin to be then type G10 L20 P2 X0 Y0 Z0. The G55 work system will then be set. Run the first job, change your tool, home it,make sure you have G55 set, then G0 x0 y0. Then drop Z down and reset Z when it's at top stock. If the origin area is carved out just reset Z on an area of stock that isn't carved out.

[keithc]

Well, I though I had that working. And I have using a WCS as stated. kicking my butt.

[aforww]

Feb 13, 2017 20:46:39 GMT keithc said:

Well, I though I had that working. And I have using a WCS as stated. kicking my butt.

Walk me through your process from homing the machine to setting your WCS. Maybe I can help you find where the fault is. I use the "return to home" button exclusively.

[markwisniowski]

Feb 13, 2017 1:46:11 GMT Derek the Admin said:

You will have to break it into two different files because Fusion generated G code is probably issuing tool change commands which grbl is just ignoring because the kind of machines grbl (the control firmware) was meant to run will pretty much never have an auto tool changer.

You can use Work Coordinate Systems to pick up the same position over and over again. Jog to where you want the origin to be then type G10 L20 P2 X0 Y0 Z0. The G55 work system will then be set. Run the first job, change your tool, home it,make sure you have G55 set, then G0 x0 y0. Then drop Z down and reset Z when it's at top stock. If the origin area is carved out just reset Z on an area of stock that isn't carved out.

I'm about to practice making a tool change on the same part I'm cutting but I have one main question about "Resetting Z".

For example, I start my first program using a 1/8" flat endmill to rough out everything, next I want to use a V-bit to trace some lines on top of my part. My 1/8" flat endmill has a red ring that tells me how far to place my endmill into the spindle collet but my V-bit does not have the ring. My initial X0,Y0 and Z0 on the part is no longer there because its been cut away...

So when I "Return to Zero" in UGS Platform the spindle moves to the original WCS point that I have placed, which is great but how do I know how deep to place the V-bit into the spindle so the tip of the V-bit is in the same spot as the tip of the 1/8" flat endmill. I can't place the V-bit on top of the part because that portion is gone now from the roughing pass.

[emac319]

You could create two different programs. The second tool will have to be touched off on the post roughing operation.

[markwisniowski]

Mar 14, 2017 18:30:50 GMT emac319 said:

You could create two different programs. The second tool will have to be touched off on the post roughing operation.

Yep, 2 different programs. Are you saying on the 2nd program that I should Return to Zero, then jog over a little bit to touch the V-bit to the top of the leftover part and tighten to the V-Bit in the collet then Return to Zero again?

[emac319]

Are both programs referencing the same xyz origin?

[markwisniowski]

Mar 14, 2017 19:12:18 GMT emac319 said:

Are both programs referencing the same xyz origin?

Yes

[emac319]

Touch of the first tool on the Raw stock before roughing. Record that number in machine coordinates in z. Once the rough is done put your new tool in. Touch off the new tool in the same xy but new z and set z0. Record that in machine coordinates. Take the difference and add that to all your z values in the second program. Basically calculate the amount of stock your removing in the first pass and then add that from the second program. Another way would be to set up another coordinate system in your model to ref the cut stock after roughing. Hope that's not too confusing

[emac319]

You could also mount a gage block onto your fixture as a reference for All programs. You would just have to know the location of that block relative to the table. Then you could touch off on the block every time in z

[emac319]

You should really try setting your zeros to finished surfaces if you can. That way they don't disappear in you

[Derek the Admin]

emac319 described one method. For a multi-tool job I like to set up a WCS, run my first program, change the tool, reset Z using an area not already roughed out. For instance, if the origin in the XY plane has already been roughed out I'll just job a little bit to the left to a nice untouched piece of stock and zero the Z to that.

If all your tools have indexing rings you can calculate the offset between them though and keep a little log. Change tools then reset the Z according to the offset.

[aforww]

Mar 15, 2017 4:54:57 GMT Derek the Admin said:

emac319 described one method. For a multi-tool job I like to set up a WCS, run my first program, change the tool, reset Z using an area not already roughed out. For instance, if the origin in the XY plane has already been roughed out I'll just job a little bit to the left to a nice untouched piece of stock and zero the Z to that.

If all your tools have indexing rings you can calculate the offset between them though and keep a little log. Change tools then reset the Z according to the offset.

This is what I do. All my tools that have indexing rings I measure and adjust the ring so that they are the same. I write down that measurement and periodically check them before I run em.