Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: kak on June 03, 2009, 05:13:10 PM
-
Hello
I`m playing with my little router milling blue foam and learning. I just made a Z touch PCB plate and it works great.
But how to zero the X and Y axis?
I used my eye and moved the X axis so the edge of my router bit was touching the material. I did the same with the Y axis and zeroed them. I was expecting to mill 1 mm around my material, but the first 2 edges was not milled, and the opposite 2 edges was milled 2mm.
Here is my milling video http://www.youtube.com/watch?v=3AXxEmQW-Ro
Is the X and Y zero not where the tool touches the material?
Can I get any help how to zero the X and Y axis? I like the PCB idea - how can I use it to zero the X and Y axis? I`ve seen it on youtube somewhere, but without a description.
Adam
-
If you touch the edge of the material and zero the DRO your zero position will be off by half the diameter of the cutter, so instead of zeroing the DRO type in the number, eg if its a 10mm dia cutter then enter -5.
Hood
-
X and Y zero can be anywhere. It is usaully depicked by the CAM or the progamer to make it easy to setup. Look at the code to determan where it is. Take into account if there is tool comp or just tool offsetting involved.
OK just looked at the vid I think HOOD has your answer (;-) TP
Just a thought, (;-) TP
-
Thanks for your answers. I will try that.
But one more thing. Is the Offset screen in Mach3 working? I don`t know anything about this VB scripts, but I`ve seen that the Edge Finder buttons has some scripts assigned.
I use the PCB as a Z axis zero tool which is connected to GND and port 15 - it works great.
But can I use the same tool to find the X and Y edges using the Edge Finder screen? And how?
Adam
-
Thanks for your answers. I will try that.
But one more thing. Is the Offset screen in Mach3 working? I don`t know anything about this VB scripts, but I`ve seen that the Edge Finder buttons has some scripts assigned.
I use the circuit bord as a Z axis zero tool which is connected to GND and port 15 - it works great.
But can I use the same tool to find the X and Y edges using the Edge Finder screen? And how?
Adam
If you look in the Files section of the group, there is a file "RayLs Probing Macros", or something close to that, that contains all the macros, and a modified screenset, to enable edge, corner, center and mid-point finding, and tool length touch-offs using that page. With the stock screenset, most of those buttons don't do much more than zero a DRO.
Regards,
Ray L.
-
Thank you Ray
Something is moving on Mach 3 screen on my home PC - without the router. Now I go to try it with my router.
I`m a metric user, and I saw you wrote something about inches - do I have to modify something, somewhere?
This PCB I use or a piece of a metal pipe as the Z zero and edge finder tool - is it enough to conect it to port 15 and have some wire connected to GND and my router bit, and mark it as a Probe in config menu?
Adam
-
Thank you Ray
Something is moving on Mach 3 screen on my home PC - without the router. Now I go to try it with my router.
I`m a metric user, and I saw you wrote something about inches - do I have to modify something, somewhere?
This PCB I use or a piece of a metal pipe as the Z zero and edge finder tool - is it enough to conect it to port 15 and have some wire connected to GND and my router bit, and mark it as a Probe in config menu?
Adam
Adam,
You do need to set Mach3 to operate in metric, but it has no effect on the macros - they use whatever units Mach is using.
For the tool length setting, all you need is a piece of PCB material with a wire soldered to the top side, and connected to the PROBE input of your BOB. You *might* need to put a pull-up resistor on the BOB end of the wire, if the BOB does not already have pullups. The tool will be grounded, so when it touches the plate, the PROBE input gets yanked low.
For edge finding, you can use the same piece of PCB material, slipped in between the tool and the part, but in that case you'd need to set the "probe diameter" DRO to the radius of the tool plus the thickness of the PCB material. This will work fine, but will sometimes be hard to get the PCB material in the right position to get an accurate reading. I use a Fowler electronic edge finder (about $30 from Enco, etc. - see Enco P/N 307-3436) that I've modified by removing the "guts", and connecting a wire to the probe tip. I made the wire short (about 6"), and put an alligator clip on it. I have the piece of PCB material permannently connect to my probe input. When I use the edge finder, I just clip the alligator clip to the piece of PCB and go to work.
Regards,
Ray L.
-
Thank you Ray
Something is moving on Mach 3 screen on my home PC - without the router. Now I go to try it with my router.
I`m a metric user, and I saw you wrote something about inches - do I have to modify something, somewhere?
This PCB I use or a piece of a metal pipe as the Z zero and edge finder tool - is it enough to conect it to port 15 and have some wire connected to GND and my router bit, and mark it as a Probe in config menu?
Adam
BTW - Make sure you configure the PROBE input as active LOW.
-
I can`t thank you enough Ray - it`s working :-)
But the Vise X - why does it touch the same side of my material twice? There is only 1 zero point.
Edge Finder: http://www.youtube.com/watch?v=XwOuTb0O1_Y&feature=channel_page
Vise X: http://www.youtube.com/watch?v=4rtn5gTvzeU
Center finder: http://www.youtube.com/watch?v=-UUwVK6FYN0&feature=channel_page
Adam
-
One more question.
Now I can zero the top of my material, but if I mill it away and I need to change the endmill to ballmill and run a finish pass - how do you do it?
My future plan is to mill a wing mould for a radiocontrol aeroplane. But if I mill the top surface of my material, I will loose my Zero.
Adam
-
I can`t thank you enough Ray - it`s working :-)
But the Vise X - why does it touch the same side of my material twice? There is only 1 zero point.
Edge Finder: http://www.youtube.com/watch?v=XwOuTb0O1_Y&feature=channel_page
Vise X: http://www.youtube.com/watch?v=4rtn5gTvzeU
Center finder: http://www.youtube.com/watch?v=-UUwVK6FYN0&feature=channel_page
Adam
Adam,
It's for aligning the vise to a machine axis. For instance, if you're setting the vise so the fixed jaw is parallel to the X axis, it first locates the left-front corner of the fixed jaw in both X and Y, and zeroes to the DROs to that corner. Then it goes to the far right-hand end of the fixed jaw, and checks where it is in Y relative to the first end. The status line displays how far out of alignment the jaw is. So, if it indicates the mis-alignment is +0.010", that means the right-hand end of the vise is 0.010" further back (towards the column) than the left-hand end.
If you've completely milled away the top face of the part, then you can re-zero to the new surface, and either adjust your code for this new zero datum, or, after letting the macro zero to the new top surface, manually re-set the Z DRO to the true Z dimension (for instance, -0.010" if you had removed 10 thou). It's also sometimes handy to set your zero reference to the bottom of the part instead, so it doesn't move if you face the entire top surface.
Regards,
Ray L.
-
Himy,
Your probing stuff looks really handy.
Where does one find the 'Files' section of the group. I'm sure it's in front of my face, but I can't find anything.
Thanks,
-
Thanks again.
Is it possible to make some kind of Offset from my "job Zero point" to a location where I always be changing tools? That will be the best way to do it but I don`t know how.
Adam
Ps. Simpson36 - its in the Yahoo Groups. Look at Mach support window.
-
Thanks again.
Is it possible to make some kind of Offset from my "job Zero point" to a location where I always be changing tools? That will be the best way to do it but I don`t know how.
Adam
Ps. Simpson36 - its in the Yahoo Groups. Look at Mach support window.
It's certainly possible - you can do almost anythig with macros. But I don't understand exactly what it is you're proposing. Ordinarily you touch off on the part to establish your zero point, then use fixtures if you want to offset from there.
Regards,
Ray L.
-
Thx, had to join that group. Waitiing to be 'approved' ::)
-
Just downloaded them and uploaded here to save you waiting ;D
Hood
-
Thanks, Hood!
Got it!
-
Sorry Ray. I just can´t understand this. I don`t know enough about cnc.
I think I will leave some part of my material unmilled, so I will still be able to Zero the top surface before the finish pass with ballmill.
I just want to make the wing mould when I`m ready for it.
Adam
-
Kak,
It's not complicated, instead of starting at the top surface and using negative coordinates, you simply start at the bottom and all coordinates are positive, which is actually more intuitive, in my experience.
'Zero' is used as a noun and also as a verb in machining, so those darn semantics get in the way again . . i.e. 'zeroing' (verb) is just a term used for the process of telling the CNC machine where stuff is and it does not necessarily involve the number zero (noun) at all.
Example: Let's say your stock is .75" . . grab your PC board and do the the tool height thing with the Himy stuff and what do you have? You have the end of the tool .75" (material thickness) plus .125" (the PC board) above the bottom of the stock. All you need to do is tell Mach3 where the tool currently is. There is no rule that says you MUST get the tool to 0.000 and then tell Mach it is at 0.0000. Mach just needs to know the coordinate of the CURRENT position and it will know where everything else it from there.
In the example, if you want the bottom of the material to be zero, then the tool is currently sitting .875" above that, so you simply tell Mach where it is by typing positive .875 in the DRO and your good to go. You do not have to have the tool physically at zero on any axis. 'Zero' (the noun) is simply a reference plane from which the coordinates are all taken. It could be on the roof or 100 feet underground.The only caveat is to remember that you physically hit something at positive .875 in our example, so don't get absent minder (like me) and pick up the tool to say .5" for a rapid move or :'(
-
Thanks simpson.
It`still hard for me to understand it, but I have only read your last post 10 times :-)
The first line you wrote about starting at the bottom - is it something you do with the CAM software or Mach3? The Gcodes starts at the bottom or the tool is touching the bottom when it´s zeroed?
Because I think that if I set the Z zero at the bottom of my material, the machine wil try to mill my table. But it can`t - thanks to limit switches.
I think my coordinates are always positiv, but I didn`t play enough with different settings.
I don`t know how the professional Cam software works, but I`m using Meshcam. If I generate the Gcodes, I can save them one by one. f.ex. first Rough and then Finish. When the rough pass is over with an endmill I load the Finish pass Gcodes, but I need to change tool to a ballmill first. The "start point" for both passes is the same, but my ballmill is maybe longer then my endmill.
And because the top surface is milled away during the roughing pass, I can`t zero the ballmill. The ballmill needs to be zeroed on top of the material surface, which is gone.
Thats where I am now, but I need to try this Zero at the bottom next time.
Adam
-
Adam, I too tend to be overwhelmed by Mach’s tool-length/offset/fixture features. There is also a simple way.
Touch off on the top surface and set the Z-DRO to zero as you describe. Now jog over to the mill table (or any other reference surface that can be used as a repeatable datum) and touch off. Write down this value.
Now when you install the ball cutter (or otherwise loose your Z reference), touch off on the spot that was used as a datum above. Set the Z-DRO to the recorded value and you are good to go.
Hope this helps,
Al
-
Zero at the bottom was just a suggested solution that I think Himy made for you. That IS a solution, but it is not a rule. There are lots of ways to skin a cat, and you have not invented a new problem. We all have the same issue to deal with. You seem to have become impaled on the 're-zeroing issue, so my suggestion is to simply walk around that obstacle and not re-zero at all.
I'll just give you a quick example of the best way to solve your problem and you'll need to do your homework from there. You need to study the tool offset feature of Mach and get yourself a couple of end mill holders for whatever spindle taper you have.
Example: you have one endmill holder with your roughing endmill. You have another end mill holder with your ball end finishing mill. You LEAVE these items together so that you change the holder/endmill together as if it were one solid piece.
Now, since the holder/endmill combination has a fixed length, you simply need to tell Mach what the difference is and it will AUTOMATICALLY compensate for you when you change tools and you do NOT have to re-zero. For simplicity, lets say the holder/roughing mill is zero, but when you switch to the holder/finishing mill and place the end on the same surface, the DRO now reads positive .25". No problemo, just tell Mach that your finishing mill is .25" longer than your roughing mill and when you change the tool, you tell Mach "changing to tool number 2 now" and Mach will automatically adjust for the longer tool.
That's all I have time for right now, but Mach has these features that are designed for exactly the situation you have, and it is invisible to the CAM program.
-
Al- it took a few minutes to visualize what you discribed, but now I can se and understand it. Thanks. That will work.
Simpson - I´ve been playing with the different tool offsets. It works, but I don`t have the tool holder.
Im building a larger router and I use the Kress spindle. I dont think there is a tool holder for Kress, but I could weld some kind of stop on all my tools and messure the lenght from there.
I know I didn`t invented a new problem. I just thought there is some kind of a smart macro doing all the job.
I like the way you explain it for a newbee like me :)"You LEAVE these items together so that you change the holder/endmill together as if it were one solid piece".
But thanks for all your help. I know how it works now.
Adam
-
Im building a larger router and I use the Kress spindle. I dont think there is a tool holder for Kress, but I could weld some kind of stop on all my tools and messure the lenght from there.
If there is no quick change available for your spindle (or if is stupid expensive), and your tools don't bottom in the collets (or however you hold them) you can still get a repeatable reference length by just putting a collar on each tool so that it installs in he same place each time you use it.
That will have the same effect as an end mill holder realtive to your tool change proceedure. You measure the tool once and tell Mach how long it is and then when you change tools, you just tell Mach which tool you are going to use and it looks up the length of that tool and 're-zeros' for you . . . is one way to view it.
The tool tables and fixtures can be a big elephant to eat for a newbee, but take it a bite at a time and you'll get it. It's worth the effort and you will wonder how you every got along without it, once you figure out how convienient it is and how much time it saves.
-
Im building a larger router and I use the Kress spindle. I dont think there is a tool holder for Kress, but I could weld some kind of stop on all my tools and messure the lenght from there.
If there is no quick change available for your spindle (or if is stupid expensive), and your tools don't bottom in the collets (or however you hold them) you can still get a repeatable reference length by just putting a collar on each tool so that it installs in he same place each time you use it.
That will have the same effect as an end mill holder realtive to your tool change proceedure. You measure the tool once and tell Mach how long it is and then when you change tools, you just tell Mach which tool you are going to use and it looks up the length of that tool and 're-zeros' for you . . . is one way to view it.
The tool tables and fixtures can be a big elephant to eat for a newbee, but take it a bite at a time and you'll get it. It's worth the effort and you will wonder how you every got along without it, once you figure out how convienient it is and how much time it saves.
Of course, a tool with a collar for a depth stop, inserted into a collet, will only be accurate to a couple thou, as how far the tool pulls up into the collet will depend on how tight you pull the drawbar.
Regards,
Ray L.
-
If he had a drawbar, he'd be able to use holders.
It seems he is using a router head or something similar, so it would likely be a collet of some type.
-
Hello everybody, this is my first post.
I have the RayLs Mach3 Macros and screensets and everything is working perfect but I need one more thing and I don't know how to do it.
If I use "Auto tool zero", everything is ok because I have a DRO for adjust the "Plate Thickness", but if I wanna use the other things, like "Edge finder", "Vise X" or "Center Finder", I don't have a DRO for the "Plate Thickness".
How can I add a DRO for that?
I'm begginer so I don't know how to do. I need some help.
Thanks in advance.