Machsupport Forum
Mach Discussion => Video P*r*o*b*i*n*g => Topic started by: CNCStone on February 25, 2019, 02:34:48 AM
-
Hello guys! I am Peter and I am stonemason and I use CNC mill for 90 percent of my jobs. I have read a lot of topics on the forum but none of them points me directly to solution of a problem:
My granite slabs are polished as glass and they are uneven on the surface. When I have to engrave a 100 or more letters on them I have to measure every two letters and make a separate toolpath in aspire or artcam. When i have a slab 1000mm on 2000mm and it has difference lets say 2mm from one side to the other and my letters are careved 2mm deep, I get no letters on the lower side and get bold (like offset) letters on the higher side of the slab. I can always try to make the slab even, but since they are polished I cannot calibrate them with a tool, because I have re-polish them after the lettering. The other way I tried is to make the slabs even by putting something under the lower part, but this also did not worked, because most of the slabs are cut and polished like and arc. So they have a "belly in the center. So I get a slab that is Z=0 in the center of XY, and Z=-2 in one corner, Z=+1 in the other, Z=+2 in the third and Z=-3 in the fourth corner.
I found that my only solution is a some kind of material flatness detection software and hardware like mach3 plugin plus a laser scanning or touch probe digitizing.
Can somebody tell me what to buy to solve this problem, that I have been struggling for a long time. Thank you all in advance.
-
Hi,
I make PCBs by isolating routing. The result is highly dependent on the PCB blank being dead flat (within a few um)
OR use Autoleveller. It is a free software utility that probes the surface and subtly varies the Z axis depth of cut to maintain
constant cut depth.
You might be able to adapt Autoleveller to your needs.
http://www.autoleveller.co.uk/ (http://www.autoleveller.co.uk/)
Smurph, one of the developers of Mach4 has heralded the upcoming release of a Mach4 feature that does something similar.
A PM to Smurph or even an Email to NFS may net you enough details that would allow you to decide whether the new
Mach4 feature would suit your purpose.
Craig
-
Instead of probing the entire slab, would you be better off modifying your machine to have some sort of floating spindle.
Look into engraving using a nose cone.
Have a read of this. https://www.johnsonplastics.com/engravers-bible/nosecones (https://www.johnsonplastics.com/engravers-bible/nosecones)
-
Thank you guys for the advice. It means a lot to me that you spend your time to help me.
I found some producer for the nosecones. I will ask them if they can solve my problem. I am not sure if they can, because I engrave the slabs with pcd tools on few passes. Don't know if nosecone is suitable for engraving hard surface on passes.
About the auteleveller, today I will also ask the guys if they can help, actually this is where I started and still don't know which is the better solution.
I will post both of their responses, so this tread can be useful for other people.
I also thought about laser scanning. I am not sure if this is a way to deal with my problem. Maybe it is not since my slabs are polished and they will have mirror effect on the laser.
-
Hi,
as I suggested ask Smurph about the upcoming contour feature in Mach4.
Have you tried to get a probe file from the Autoleveller software. I would recommend AoutlevellerAE, it produces
a probe file and THEN corrects the code.
Autoleveller software is open source, you can download it and see how it works.
-
Autolleveler is going to be the first thing that I will try these days. May I ask if somebody can recommend me a good touch probe? For now I have none experience with them.
-
Hi,
with Autoleveller you present a Gcode job for the PCB. Autoleveller inspects the Gcode file to determine the
extents of the machined area and then proposes a Gcode file to probe the enclosed surface area in a rectangular
pattern. You might specify that you want probe points no more than 5mm apart so it will generate a Gcode file
that will drive a probe in that pattern and record the results.
I imagine if you present a Gcode file but instead of PCB tracks letters to be engraved then Autoleveller will
happily determine the extent of the letters to be machined and generate a probe file automatically.
I rather doubt you need an expensive probe. I would have thought a small button type switch with a stem on in that
you could mount in your spindle. If you glued a short extension onto the button and had the two wires from the
button terminals to your BoB that would be enough. Is precision beyond 0.1mm-0.2mm required? Thus you could
make a probe for under $5.
If you use AutolvellerAE the data produced by all the probe points is put into a file which gives a colour rendering
of the surface. Thereafter Autoleveller will take your original engraving file and modify the Z cut depth to match the
surface contour. That modified or corrected file is the one you use to cut the letters.
Craig
-
Craig, the precision more than 0.1 mm-0.2 mm is not required. I will search the net or even in my country for a probe and star testing immediately. I am asking you for the a probe ideas, because, those I found in my country are some very expensive, around 1000 euro... And now you telling me 5 usd will do. So maybe I am searching for the wrong thing. I will search again and post what I found. Or maybe for fast result and delivery I should try ebay.co.uk. From there I will get the probe in a few days. Should I search for a "touch probe" or for "touch probe digitizer"?
Again thank you for helping me.
-
Hi,
I wouldn't buy anything, I would make something simple and cheap. Prove the idea befoee
I spent anything.
Craog
-
Try this design, cheap enough :)
http://gtocs.blogspot.com/2012/04/garys-diy-cnc-touch-probe.html
;)
-
Hi,
my idea was for something simpler still. This is a good quality microswitch with plenty of overrun:
https://nz.element14.com/honeywell/bzc-2rq1-a2/switch-basic-top-pin-plunger/dp/1525197 (https://nz.element14.com/honeywell/bzc-2rq1-a2/switch-basic-top-pin-plunger/dp/1525197)
My suggestion is to make a small carrier like that pictured with a stem that mounts in your spindle.
Fit the switch (plunger downwards obviously) to the carrier, fit the assembly to your spindle.
You might like to glue a small extension to the plunger to have the body of the switch somewhat further away
probed surface.
Craig
-
Hi,
one of the problems with the more normal CNC spindle mounted probe is the lack of overtravel.
When your Z axis is descending looking for a contact there will always be a bit of overrun. Provided your descent
speed is not too fast and your controller operates both correctly and quickly (within a few tens of micro seconds)
the overrun will be small.
If however your controller does not respond quickly you risk burying your expensive ruby tipped probe into the surface.
Without overtravel its going to get broken.
The switch I linked has a minimum overtravel of 5.5mm.
Lets say you specify (in Autoleveller) the safe height above the nominal 'flat' surface of 5mm. You can also direct
Autoleveller to probe to a maximum depth. Thus if you caused Autoleveller to produce G31 commands of the type:
G31 Z -5.0 F100......then even if your controller missed the probe event the machine will stop its descent at -5.0mm hopefully
just a little short of the overtravel of the switch.
Craig
-
Hi
Google high precision micro switch
https://www.google.com/search?q=high+precision+micro+switch&rlz=1C1ASUT_enAU791AU791&oq=high+precision+micro+switch&aqs=chrome..69i57.12774j0j8&sourceid=chrome&ie=UTF-8 (https://www.google.com/search?q=high+precision+micro+switch&rlz=1C1ASUT_enAU791AU791&oq=high+precision+micro+switch&aqs=chrome..69i57.12774j0j8&sourceid=chrome&ie=UTF-8)
Omron have a good range
https://www.google.com/search?q=high+precision+micro+switch&rlz=1C1ASUT_enAU791AU791&source=lnms&tbm=isch&sa=X&ved=0ahUKEwj2wPHTsdrgAhVYb30KHV2QAjIQ_AUIDigB&biw=1174&bih=493#imgrc=e3unll0hLvCuPM: (https://www.google.com/search?q=high+precision+micro+switch&rlz=1C1ASUT_enAU791AU791&source=lnms&tbm=isch&sa=X&ved=0ahUKEwj2wPHTsdrgAhVYb30KHV2QAjIQ_AUIDigB&biw=1174&bih=493#imgrc=e3unll0hLvCuPM:)
If there is a risk of over travel damaging the switch place it in a spring loaded plunger that will allow it to move up and protect it from damage.
For the resolution you need it should cost less than $100
Regards
John
-
https://www.digikey.com/product-detail/en/c-k/LCS012P00WA26AY/CKN11533-ND/8536760
This switch is rated for low current, it has gold flashed contacts and is IP67 - Dust Tight, Waterproof.
-
Hi,
For the resolution you need it should cost less than $100
I would hope to do way better than that. As it turns out I have several of these switches lying around surplus.
Even if I had to buy one, the price is $20.77 NZD including GST (new Zealand sales tax). That works out to
$13.90 USD. Element14 ship free if you order a minimum of $45 NZD. That's why Element14 is my favourite
supplier.
Craig
-
Hi,
I can and have bought from DigiKey but they have a minimum freight charge of $35 NZD +15% GST.
So despite the switch you have linked to being cheap the freight kills it.
Craig
-
Hi,
apologies for the picture I posted earlier, I didn't check it out before I posted it......its way to big.....and I hate
that, a real bunnies mistake.
Craig
-
There are many suitable switches, but be sure to get one rated for low current. High power appliance switches sometimes need the high current to keep the contacts clean and can fail when used on low DC current.
Switch failure is a reason to use a normally closed switch so a dirty contact or broken wire would not cause a crash.
-
Hi,
There are many suitable switches, but be sure to get one rated for low current. High power appliance switches sometimes need the high current to keep the contacts clean and can fail when used on low DC current.
That is true. The Honeywell switch I linked to has silver contacts and would ideally be switching rather more current
than the gold contact one MN300 linked to. Having said that I have used these Honeywell switches (Omron make identical units)
for years at low currents without difficulty.
As MN300 comments there are any amount of switches that would work. I think however that plenty of overtravel is
the critical characteristic rather than switch current.
Either way the simple idea of a spindle mounted carrier should enable OP to make a probe for way less than buying one.
Craig
-
Overtravel could be accommodated by spring mounting the switch. Something on the order of a spring mounted tap follower that extends to a hard stop.
As Joeaverage says, you can often get away with using a high power switch that has never seen AC current. Higher power can mean higher mechanical operating force.
-
Hi,
Overtravel could be accommodated by spring mounting the switch
Agreed, at the cost of complexity, but entirely possible.
These (Honeywell/Omron) switches have a 'sensitive' version and a standard version. The standard version has
according to the spec I posted, a max operating force of 3.61N, equivalent to 361 gram force. The sensitive version
reduces that to about 100 gram force, still not feather weight.
Either 100g force or 360 g force is not going to upset a granite slab at all!
Craig
-
Hi,
this afternoon I downloaded the current latest development build of Mach4. It has the new surface mapping
feature and I've been experimenting with it. I haven't had anything like the time to work out all the quirks yet
but this could, in fact almost certainly, be a worthy alternative to the Autoleveller solution.
I have attached a picture of the Surface Mapping generating screen. Note that it is in Machine coordinates and may
require a certain amount of thought before banging in some parameters.
The up shot is you program the X and Y extents of the area to be mapped, the target resolution between the sample points,
the probing speed, the Z axis retract height and the vertical Z probe movement the hit <Map Surface> and Mach obediently
probes the entire area and saves that as a map file. The mapping generator is a Wizard....too easy!!
I have yet to work out how Mach handles the results of the file, but it looks like you select the surface map file
in the Surface Map plugin and thereafter the Z axis machine coordinate Z datum goes up and down automatically.
So unlike Autoleveller you do not have to modify the Gcode to accommodate an uneven surface the datum goes up
and down instead.......how bloody clever is that!!
You might like Mach3 but you are being left behind BIGTIME!, get with Mach4, go mad early and beat the rush! ;D
Craig
-
Hi,
just found the video that has just been released to show how it works.
https://www.youtube.com/watch?v=M4o6dfQrAo8 (https://www.youtube.com/watch?v=M4o6dfQrAo8)
This looks to be perfect for OPs needs. It is Mach4 but it does the business.
Craig
-
Ok. So... Tomorrow I will go to a omron shop near my city, or maybe call them on the phone today to check price and availability. The switch will be found and bought, hopefully. I am getting the idea of what I need. Low current, sensitive switch. After this I will make the mounting bracket. So the thing is that I have to decide what to use, and since the autoleveller is free I will try it. About Mach4, the feature that Craig linked a video, was the first thing that caught my eye, when I was searching for a solution to my problem. It looks nice and easy and just the thing for my need. But, I am using parallel version of Mach3 on win XP, and I have no idea if the transition from one to the other will be smooth. Otherwise I am ready to pay for Mach4 license and parallel port plugin - 225 USD in total. Just wasn't thinking of doing it now, but as Craig said maybe I will go mad and beat the rush :)
Again thanks to everybody for the will to help.
Peter
-
Hi,
Otherwise I am ready to pay for Mach4 license and parallel port plugin - 225 USD in total.
No, I think that is a mistake, the Darwin plugin/motion controller is 'to have a play' with Mach4. This is likely
to end in you having a difficult time making the transition and lose paying work as a result.
If you are serious you need to go the whole way and get a good motion controller and ideally Mach4Industial.
Projected cost Mach4Hobby/ mid-range motion controller/BoB =$500-$600
Projected cost Mach4Industrial / mid-range motion controller/BoB = $1700-$1800
There are several reasons:
1) A vastly increased range of PC's which can be used
2) Hardware/firmware support direct from he manufacturer
3) Mach4Industrial gives you one on one phone support
These combine to mean you get the easiest transition to Mach4 and maximum gain in profitable functionality
for years to come.
If you required a repair to your work vehicle of $500-$600 or even $1700-$1800 would you pay it? I imagine
that you would be hard pressed to earn a living without a work vehicle. Does your engraving mill fall into
the same category?
Craig
-
A search of nz.element14.com found this switch. 2.7 mm overtravel.
https://nz.element14.com/omron-electronic-components/d2qw-c003h/microswitch-spst-no-0-1a-14vdc/dp/2113271
-
Hi,
another useful alternative for a switch.
I notice you searched the NZ website but Element14 is global so search results are identical to any other site around the world.
The NZ site quotes prices in NZD, including GST, it also estimates the delivery from our closest warehouse which is in Sydney
Australia.
If the part is in stock in Sydney, I can order it up till 3pm and have it the next day. If my order doesn't qualify for free
freight that will cost $14 +GST NZD or $10.80 USD. I can't complain about that service!
Craig
-
I searched the NZ site because it was used in a previous post. Element14 has many aliases, Farnell in the UK and Newark in the US. I favor Digi-key because their main location is only 300 miles away.
The surface mapping video shows some very rapid probing with what appears to be a rigid probe so I wouldn't worry too much about overtravel. It wouldn't take much experimenting using the MDI to find the amount of Z axis travel past the probe sensing point for various Z axis speeds. Then you could select a fast but safe speed.
-
Hi,
The surface mapping video shows some very rapid probing with what appears to be a rigid probe so I wouldn't worry too much about overtravel.
It was only done at that speed for the video. If you are not concerned about overtravel that's fine. I however have done a lot
of probing on PCBs and found that a probe which has overtravel saves crashes.
Craig
-
Hi,
I have given considerable thought to overtravel and have done my best to quantify it:
https://www.machsupport.com/forum/index.php?topic=38730.0 (https://www.machsupport.com/forum/index.php?topic=38730.0)
Craig
-
Hi to everybody! I will make something like double post.
First, to Craig about the car and the cnc mill. Yes I need both for my work and I make some money thanks to them.
Second about the switch, I bought one omron switch, and going to make something like Craig sketched in the beginning of the tread. Then I will try with autolleveler and see what is going to happen.
-
Hi,
kool! This is a simple and cheap way to try it out. Having used Autoleveller I am confident that you could use it
to advantage, and even better, for next to no expense.
Should it prove otherwise or for any other reason you chose to try Mach4 then do yourself a favour and get yourself a decent
US or European external motion controller and be prepared to spend a few hundred on it.
Mach4 was and is intended to be complemented with such a controller. Mach4 has progressed to the point where it matches or in
some cases well exceeds Mach3. It is easier to transition from Mach3 to Mach4 than it used to be but is still far from trivial.
You would be commended to download Mach4 and run it in Demo mode, for free, until you are ready.
If you have not used an external controller before it will cause quite some confusion as to how they work together
and where one hands off to another. Thereafter however the Gcode and operation of Mach4 is very similar to Mach3.
The second learning curve is if and/or when you want to start modifying Mach4 to some specific need of your own.
It is very capable of such modification but is a steep learning curve. Fortunately 99% of Mach4 operations require no
such modification at all.
Let us know how you get on with Autoleveller.
Craig
-
Second post.
So look what a friend gave me.
https://www.keyence.com/products/sensor/fiber-optic/fs/models/fs2-60/index.jsp?search_dl=1
He told me that this is some scanning device from a 3 axis cnc from Italian company Marmo meccanica.
It is a digitizer in his opinion, but the machine is unknown, he bought from an auction and there was no more information about the device and the machine.
There is something I found in another company portfolio and attached a picture.
My question is - has someone seen and used something like this on his CNC? Is is possible to adapt something like this to Mach with third party software? I am just curious.
-
here are the pictures
-
Hi,
the first picture declares the device is a go-nogo unit for tracing the outline of a template.
I don't think therefore that you could call it a scanner in the sense that it can produce a 3D point cloud.
In fact I don't think it can measure distance at all, therefore it might be able to assist in scanning an object or template
that would allow a 2D outline of the object to be produced but not its Z height.
Craig
-
Again thank you Craig, for helping the noobs like me. Until I am ready to do some tests of my probe, which will be next week, I want to ask an off topic question.
A friend of mine is building different kinds of machines and he is going to build me a new cnc machine with my financial and physical help. The CNC will have forth axis - "A". I still want to be able to do measuring with probe, not that I had done any, but I believe I will. So me question is:
- Should I make the machine with mach3, because of the customization possibilities and the third party software that you can install on the windows pc, or should I choose something else.
He told me that we can use DSP, Syntec, Mach. He is more of a mechanic and less software guy. But he helps me a lot.
So to make it more clear. What controller should I use for 4 axis cnc and should I use mach3 or maybe mach4 just for the customization that I can always make, like the probing that we are talking here?
Hope that I wrote it understandable.
-
Hi,
you will have to decide whether you use a Windows PC at all. Windows PCs are not realtime so the motion controller
has to handle all the realtime activities. As a consequence the abilities of the motion controller have a great deal of
influence over the machine behavior.
LinuxCNC is very capable alternative, and is predicated on several distros of Linux that have Real Time Extensions,
meaning your PC (no longer Windows) becomes a realtime machine. You can use a parallel port rather like Mach3
or you can use Mesa cards which extend the parallel port. LinuxCNC is open source and is ultimately very flexible
but that requires some programming ability.
Mach3 was always one of the go-to Windows based software solutions and that was predicated on the use of Mach's
parallel port driver. It was cheap and capable and generated a huge user base.
Nowadays the parallel port, while still free, is looking increasingly like an antique and external motion controllers are
the norm.
This has bought Mach into competition with UCCNC, another capable software solution.
Reluctance of users to take up Mach4 has resulted in many previous Mach3 users going to UCCNC.
It would pay to do your own research.
If you still favour Mach then for a new machine I would go for Mach4. As I have posted before Mach4 all but requires an
external motion controller. Budget $500-$600 for Mach4Hobby and an external motion controller and BoB(s).
Craig
-
Hi,
I dont want to use windows pc, but it is the most flexible platform, for further development in time.
For now, I just need controller that operates with four axis, and have probing features for the uneven material that I work with. I thought that mach is the only way for me. Now I see UCCNC and see that there more and more alternatives.
What would any of you, use for this kind of job?
For the old machine, I am going to do the probing/ digitizing with mach3, and hope to succeed.
For the new machine I begin to wonder what should I choose?
-
Hi,
just about any decent external motion controller will offer four axes.
The UC***** series from CNCDrive are required for UCCNC but are also applicable to Mach.
Craig
-
http://shop.cncdrive.com/index.php?productID=965
This looks interesting and if I understand, I will be able use it also with mach3. This looks like a good price even to test it on my old machine.
-
Hi,
the AXBB controller has just been released, I'm not sure that it has a Mach3 plugin yet.
Check with CNCDrive if it is your intention to use it with Mach.
The older UC100, UC300 and UC400 all do have a Mach3 plugin and so you could use either Mach OR UCCNC.
Craig
-
Hi,
I think I have decided for to use mach4 for the new build. Now I have a few questions...again...
1. Craig are you using mach4?
2. Can I use mach4 for my 4 axis machine? I mean is it stable with four axis?
3. If I invest in mach4 industrial, I will be happy. But, I read some topic about the hobby version having the probe functionality, and the industrial only having preparation for installing macros from companies that sell probes. Do not know if this is real news.
4. If I pay for industrial, I need to get a good controller and BoB. What would you guys suggest?
5. What pc should I aim for. Motherboard? Memory? Video? Ssd? Windows 10? Processor?
Sorry for the tons of questions, I am really a noob, but I want to leaen. And for my work I really need four axis and surface mapping...
Thank you all in advance,
Peter
-
Hi,
1) Yes, have been using Mach4 for a little over 2-1/2 years.
2) Yes, Mach4 can handle six coordinated axes (plus Out-of-Band axes as well up to a total of 32 motors).
3) Both Industrial AND Hobby handle probing identically.
and the industrial only having preparation for installing macros from companies that sell probes.
I've never heard of that.
The only feature that Industrial offers that Hobby does not
is Macro B programming. It has some application in industrial programs, things like conditional Gcode and stuff like
that. Have a look at Cbyrdtoppers (Mach4 board) description of how he used it for his grinding machine. If you have
been using Mach3 and it works for you then you wont need (or miss) macro B. The real advantage of Industrial is
SUPPORT. You ring NFS and you go to the top of the queue.
I am not aware of anything that obligates you to buy
Industrial but note that the Industrial licence applies to ONE machine only. Hobby on the other hand can be used
on up to five machines. It might be worthwhile explaining your situation to NFS. It may not be unreasonable to start
with Hobby and if it goes well for you then get Industrial, maybe NFS can do some sort of upgrade?
4) With either Hobby OR Industrial you need a good controller. Remember that the controller handles ALL the realtime
functions so no matter how good Mach is (or isn't) the controller determines how the machine will behave.
I personally prefer the Ethernet Smoothstepper by Warp9 TD. It is moderately priced ($190), not the cheapest but not
the dearest either. Just recently a number of new realtime features have been added (backlash comp, lathe threading,
and encoder driven PID spindle control). The long awaited THC feature is due to be released in a few days. That makes
the ESS the most up-to-date controller in the moderate price bracket.
Other worthy contenders are the 57CNC by PoKeys, the PMDX-424 by PMDX, the UC300 by CNCDrive.
One of the more expensive ($600) offerings is the Hicon by VitalSystems. It has always enjoyed an reputation of having
well developed realtime features. Until just recently it was the only controller to offer realtime THC for instance.
Another extremely high quality offering are the motion controllers offered by Galil. For four axes they start at about $2000.
The Galil, Hicon, PMDX-424 and probably the 57CNC don't require a BoB whereas the ESS and UC300 do. I would recommend
the modestly priced ($23) C11, one only for a simple machine but two (or more) adds much more IO. You will have to make
a few simple additional circuits to 'flesh the C11 out', or buy a more expensive BoB. CNCRoom does an MB2 especially for
the ESS, all three ports are developed to be used and connected to the outside world. It is about $200.
5) I use a dual core (1.8 GHz) Atom mini-ITX board, with NO graphics card. Its a really low powered board but it works really
well. Its slow if I load really big etching files (10M plus) but once it loads and draws the toolpath it goes great guns
thereafter. The real advantage of using an external controller is that just about any 'cheap as chips' PC will work. Check
this little sucker out:
https://www.dfrobot.com/product-1585.html (https://www.dfrobot.com/product-1585.html)
$209 with 4G/64G and Windows 10 Enterpise already loaded.....hard to beat that value and less than 4 inches square!
To accommodate Mach alone Windows 10 with 4G RAM and 64G hard drive would be ample. A graphics card is recommended
but I don't have one on my machine so I hardly rate it as essential. i3 or i5 is any amount for Mach.
If you want to load CAD/CAM on the same PC ??? then up the ante in the processor/memory/HDD/SSD/graphics to suit,
Mach doesn't require it but CAD/CAM do.
Craig
-
Hello guys! I am Peter and I am stonemason and I use CNC mill for 90 percent of my jobs. I have read a lot of topics on the forum but none of them points me directly to solution of a problem:
My granite slabs are polished as glass and they are uneven on the surface. When I have to engrave a 100 or more letters on them I have to measure every two letters and make a separate toolpath in aspire or artcam. When i have a slab 1000mm on 2000mm and it has difference lets say 2mm from one side to the other and my letters are careved 2mm deep, I get no letters on the lower side and get bold (like offset) letters on the higher side of the slab. I can always try to make the slab even, but since they are polished I cannot calibrate them with a tool, because I have re-polish them after the lettering. The other way I tried is to make the slabs even by putting something under the lower part, but this also did not worked, because most of the slabs are cut and polished like and arc. So they have a "belly in the center. So I get a slab that is Z=0 in the center of XY, and Z=-2 in one corner, Z=+1 in the other, Z=+2 in the third and Z=-3 in the fourth corner.
I found that my only solution is a some kind of material flatness detection software and hardware like mach3 plugin plus a laser scanning or touch probe digitizing.
Can somebody tell me what to buy to solve this problem, that I have been struggling for a long time. Thank you all in advance.
G-CODE RIPPER (freeware) + a very simpe z-axis probe
http://www.scorchworks.com/Gcoderipper/gcoderipper.html
Can already solve a problem like yours.
** G-CODE RIPPER Now with "Auto Probe" for cutting (+ engraving) on uneven surfaces **
-
Hi,
yes Gcode Ripper could be an excellent solution. The Autoprobe feature of Gcode Ripper is very similar to
Autoleveller. I even have some little input into it myself, two macros, m40 and m41, were written by me in Lua
for using Autoleveller with Mach4 and subsequently adapted to add Mach4 support to Gcode Ripper.
Craig
-
There is also a feasible mechanical solution to engraving on Granite slabs.
NO NEED FOR any PROBING & AUTOLEVELER SOFTWARE even.
The engraving spindle head is mounted on additional rods and linear bearings so the head will move up and down freely but will drop to lowest by its own weight by gravity. The engraving head has a smooth nose ring that that will glide on the surface of the granite and the engraving tool will only engrave the depth between the it and the nose ring - a consistent depth of engraving always.
Z axis motor do still move the head up and down but the actual depth of cut is NOT actually controlled by the z-axis motor.
(I learned this from Multicam CNC machine builder about 20years ago at their factory)
Not hard to implement on the z-axis of a typical CNC router. Just decouple the z: motor from the spindle mount and make it LIFT the spindle from the bottom only.
Then
modify (lock the springs) of an "auto pressure foot" to suit.
-
Auto pressure foot has bearings to glide
-
Ok I made this /the attached picture/ , based on Craig's drawing and from what I saw on the videos for Gcode ripper. I just made some mistakes and cannot mount it on the spindle head, but I will change the mount will be ready soon.
The flexible spindle mount or the spring nose cone are both very cool ideas, but I engrave the granite slabs on passe. For example if I need 5 mm deep engraving, I make 10 passes of 0.5mm. otherwise the pcd tool brakes.
-
"The flexible spindle mount or the spring nose cone are both very cool ideas, but I engrave the granite slabs on passe."
This is the theory:-
The nose ring will only determine the final depth say 5mm (ie. the last 1 or 2 passes) when the z: motor is by then be lowered a little more lower than 5mm below surface so that the ring would then determine the final depth.
Before the final 1 or 2 passes, the z: motor could still be engraving 0.5mm at a time for 8/9 times since the nose ring would NOT be touching any surface as yet.
Of course the feasibility would depend on how even/uneven or how level the slaps are loaded. Is a spirit level used?
If this method can be made to work, it may save the time needed to do probing.
Saving time can mean saving money and increasing profit.
-
Cutting granite makes stone dust. Will sliding a ring across the dirty surface make scratches in the polished surface?
-
Cutting granite makes stone dust. Will sliding a ring across the dirty surface make scratches in the polished surface?
I think that is a very good point.
An air jet or vacuum to clear the stone debris (before it reaches the ball bearings set in the ring) may be good.
-
Cutting granite makes stone dust. Will sliding a ring across the dirty surface make scratches in the polished surface?
A dust chute for the auto pressure foot may help.
(This I made myself)
-
That's it, just the thing :D
-
The sliding ring may not work for all applications. Sometimes the background may be cut away leaving the lettering. Then there may not be enough supporting material for the ring.
-
Agree.
"Horses for courses"
-
:)
-
Hi,
I imagine the tool would be flood cooled. Water cooling vastly extends the tool life, poly crystalline diamond tools
are expensive.
Craig
-
Maybe think of other ways if Diamond bits are very costly
FYI
A small factory in Sydney invested in a 10 feet x 20 feet 5-axis CNC waterjet and was able to replace a hugh CNC DIAMOND circular saw, a huge diamond wheel CNC grinder, 3 SKILLED craftsman using air powered diamond circular saws/grinders.
Business is dealing with large
Marble slabs, Granite slabs, fake granite slaps, terracotta etc.
5-axis CNC waterjet use just pressurized water + fine sand to cut, chamfer or roundover the cut edges, and can even engrave (which 3-axis waterjets can't).
He even contracted a sign maker opposite his factory to cut metal and plastic signs for them - replacing their CNC routers.
I was there for two weeks when the waterjet was being installed and tuned up.
A small suction (fork) lift and a suction crane load and transport the slabs on/off the CNC waterjet. Little off leveling is automatically compensated by the waterjet auto probes before the g-code actually start cutting.
Computer is embedded industrial Win XP with 3 parallel ports controlling servos and pumps etc. etc.
-
Hi,
I bought a Harvey Tools (high quality if pricey brand, superb selection) 0.5mm PCD endmill.
If memory serves it cost about $78US but by the time it was shipped to New Zealand it cost me $250NZD.
You can be sure that when I use it I KEEP IT COOL. Of course being so small its very tender anyway.
The point is that you can turn a $300US PCD tool into a few dollars worth of scrap by letting the tool overheat.
On the other hand that same tool will last hundreds of hours if you do keep it cool.
OP has obviously been using these tools for a while and presumably making money doing so. For the sake of
a $20 home made probe and some time to experiment with Autoleveller, Gcode Ripper or Surface Map (Mach4 only)
he can improve what he is doing WITHOUT spending big bucks.
Craig
-
Hi.
About the cooling, well yes I use pcd, vacuum brazed, electroplated, sintered diamond tools. They all need a lot of water to "stay cool". :)
On the topic for the auto pressure foot spindle mount. I was thinking about buying one. There will be no problem for the bearings sliding on the material, if they are aluminium or poliamid. BUT as MN300 wrote, there is the problem with removing the background around the letters, which is the main method for engraving in my region. I believe that the engraving will mess up when it starts to work on area where all the background is removed and also the marble pieces that will be left behind from the material will be carried around from the bearings on the polished surface.
About the surface mapping. This is an interesting topic. I will try do some next week. From what I saw on the hundreds of videos that I watched, I think that the mach 4 feature will be most suitable.
The reason behind my thoughts, is that most of my projects are made by few different tools. For example, I use pcd for the clear contour of the letters - this is one g-code, and after that I use vidium tool to remove the background - second g-code. So if I need to make the scan over and over with each tool (each g-code) it may cause differences and loss of time.
What I am saying is that I haven't tried autolleveler or g-code ripper yet. And I am not sure if there is a way on both of them to make a tool change without having to re-scan, the surface.
The g-code ripper has a nice feature - the offset of the probe from the tool. Not sure if the others have the same function.
https://www.youtube.com/watch?v=QN8yPjy6uTk
This video gave me the idea to make a permanent mount for the probe on the machine. So if I don't need to change the tool between the different jobs, I will not need to put the probe on the spindle. The probe will stay there on the machine and will wait for doing what its made for.
Thank you all for the ideas, it is really great to get some advice when you do something you haven't done!
Peter
-
Hi Peter,
What I am saying is that I haven't tried autolleveler or g-code ripper yet. And I am not sure if there is a way on both of them to make a tool change without having to re-scan, the surface.
I haven't used Gcode Ripper so cannot comment on that but I have used Autoleveller a lot. I have only experimented
with Surface Map only sufficiently to get a feel for how it works.
If you use AutolevellerAE per my recommendation then it will create a Gcode routine to probe the surface prior to any
engraving. The data that results from that probing sequence is stored in a file and if you like gives what amounts to
a topographic map of the surface. It also generates a colour map of the surface to give you a feel for the flatness
or otherwise of the surface.
When you apply the Autoleveller correction routine to the Gcode of your engraving file is re-writes the Gcode with subtle
changes in the Z axis to reflect the underlying surface. If you need to run two engraving files to complete the job
then both would be processed similarly without probing in between.
Some of my PCB routing files require multiple tools (wear and breakage). This can be accommodated by Autoleveller as there
is one reference location that you can jog to and touch off a new tool before restarting the job to carry on from where the
previous tool failed.
Surface Map is only slightly different. The surface is probed and stored in Mach. All subsequent moves are made with the Z
axis datum going up and down automatically. If you need to run two files that's fine, the sbtle variations in the Z datum
are the same for both files, no need to probe in between.
I would recommend mounting the probe in the spindle chuck. Otherwise your probe point will be displaced from the position the
tool will be in when the job runs. Its a pain taking the tool out, fitting the probe, running the probe file and then refitting
the tool, but that's the way it has to be.
Craig
-
In "gcode ripper", after the offset of the probe and the spindle is known, every correction is automatically calculated. So the probe need not be in the spindle but just mounted permanently somewhere on the spindle mount.
-
Hi,
that's a kool idea. To my knowledge that is not possible with either of the other two solutions.
Craig