PDA

View Full Version : CNC milling glass



ckirchen
08-11-2007, 02:07 PM
Hi all,

A customer of mine has asked me if I can cut glass for him. It's 3mm annealed float glass and the final shape is a 6" x 15" rectangle with 3/32" corner radii and a 0.05" x 45° chamfer around the outside. He would supply the pieces waterjet cut to +0.025" per side larger than finished size.

He's found some diamond tools (www.winter-diamantwerkz-saint-gobain.de/database/dbfiles/partner-6/cnc_kanten_e.pdf) that look promising. I would like to use one of their shaper wheels (top of page 3) to finish the perimeter and cut the chamfer at the same time.

My machine is a CNC VMC with an 8000 rpm spindle, a partial enclosure, and flood coolant. I will likely hold the stock on a vacuum fixture to get at all four sides in one setup.

My questions:
1. I'll use the Ø120mm tool to keep the speed at 3200 rpm; what will the (flood) coolant and glass swarf do at that speed? Will it atomize and fill the shop with a glass/goolant mist?

2. I imagine I will need some kind of filter to keep the glass swarf out of the coolant tank. Any recommendations?

3. What kind of feedrates can I expect?

I'm hoping that someone has been down this road before and can give me an idea of what to expect so that I can decide whether to take the work or to pass on it. The order would be for 1500 pieces and that's a lot of time in front of the machine if my equipment is not right for the job.

Thanks in advance,
Chris Kirchen

jp3
08-17-2007, 09:13 PM
Maybe I can help, I fabbed glass for 15 years. First, thats a pretty big tool
you got there. We used 4" ish diamonds on bridgeports to bevel on side at a
time on a rectangle/square one side at a time and then set up radius jig to do
radius by hand. No fun. Then we got a milltronics cnc with a 50k spindle, and a sabre500 with a spindle similar to yours.Too bad the milltronics rarely went above 12k. Too much runout on tooling. After that we ran MANY parts just like yours on the cnc. Glass was usually cut .125 " over. Used a 80 grit(+/- 20) bonded to metal form for rough typically .5 or .375 diameter tool at between 8 and 12k rpm to rough it to . Finish tool usually same diameter 120 or 180 grit if chip spec/finish not critical, 220 grit bonded to metal form for tight specs,very rarely above 220. Bevel tools usually 1" diameter at the top 220 grit. Usually left .03 to .05'' for the finish pass depending on chip specs for O.D, bevel would have been one pass. As far as coolant water works in a pinch but there are (expensive) coolants specifically for glass. As you probably know grinding with no coolant returns glass to its elemental form :). coolant placement was tricky. you need fair amount of pressure right in there at diamond glass interface but nothing unreasonable. Spray was never a problem but you will get a little misting. After 15 years of it I'm pretty sure the inside of my lungs are white but then I did a lot of hogging with a blanchards and lathes too but cnc was never too bad with spray/mist/mess. Your 4" tool might throw some coolant around though. Used coolant filters in some apps due to scratct/dig specs but they are problematic. 10 to 40 micron typically. Funny, we ran out often and skipped the filter and it doesn't make a big difference. Swarf will settle to the bottom very quickly and harden like cement. Thats when you call a chip sweeper over to dig the tanks :) Particle size will inform your decision. 60 grit will make what almost looks like chips of glass. A 220+ grit will make baby powder and will stay suspended a longer. Spray the chuck off before and after every part and rinse part and you won't have any problems. Avoid sliding glass like the plague. Used to stack them on a cart horizontally and shake a little of what looked like fine sawdust between each part. I used to use my finger to push up on finished part to brake seal and spray water into chuck glass interface and part will sort of hydroplane up then lift off. Feedrates: wish I could give you exact numbers but that's the one thing that is a little fuzzy for me right now. It's been 8 years. Fuzzy probably because there is a lot of tweaking and variables. I think I remember doing a 4x6 1/4" thk part with a small 45 degree chamfer on the four corners and a 45 degree bevel on top in about 6 minutes or so. Thats three passes. rough OD, fine OD and bevel. Manual tool changes. Only took 10 seconds per tool. Sabre was full auto and more robust spindle so shave a minute or two off time for that.
Your only taking off .025 on the OD and .05 bevel. Don't quote the job on this but i would think you could do this part in under six minutes. You could save time with a two or four part chuck. Did two parts per load on the milltronics. four parts in a load on the sabre. Vacuum will limit feed rate. Part will push off
chuck if you feed to high ( tell you something you didn't already know right )
Used something that looked like electrical tape but was more of a static cling,
comes in wide rolls, covered aluminum vac chuck and used a razor blade to make appropriate cutouts for vac. This stuff seemed to help both seal and slip. Want something with high enough C. of Friction but not scratch or dig glass. Segmented tools are usually bad news on mills. Work great on a blanchard though. diamond bonded to metal form tools go quick. rate will have to be tweaked as it wears. Much cheaper than the big resin bonded diamonds that your looking at though. Resin bonded usually needs dressing. Brownstone if you can find it. I think I've gone on too long and yet haven't even scratched the surface. If I find an old tool I'll post some pics.

jp3
08-17-2007, 10:18 PM
Wow. I can't believe I actually saved this stuff. Now that I see the tooling I guess we might have used the 180 1" tool as well but probably on the larger cnc. Spindle quality will determine that. Point is we had access to every possible type of tool and we had best success with smaller diameter tooling for jobs almost identical to yours. Made tens of thousands of parts with this type of tooling. I just noticed you said 3mm thk. I was thinking double which is 6mm.
Should be even quicker then. Start at the bottom of the tool and when it starts to wear bump it down about .125 to get fresh diamond. Should get several levels out of one half inch length tool, double that in a one inch high tool.

jp3
08-17-2007, 11:08 PM
Ok, last reply I promise. I just read thru that German tooling catalog and had a good laugh. Reps and other assorted peanut gallery members will talk to you about ridiculous spindle rpms (20k+) until their blue in the face. And it sounds great in theory. Thats why we spent a small fortune on a 50k spindle. Never used it. You would think a diamond manufacturer would know right? Wrong. They don't. 8k might be a little on the low side but you can make it work. Get one of the tools I showed in the picture and a couple of single or double thk pieces of glass from ace hardware and you can easily prove it to your self.
last but not least, cheap mask might not hurt if you have to stick your face in there. Plated form tools use nickel and the resin bond usually use other heavy metals in the bond matrix. You can find tooling on our continent as well although the German stuff is good. I'll leave you with the sound advice I once found on a box of German diamond tooling:
!Attention! Avoid traumatic contact between diamond and workpiece.

jp3
08-19-2007, 12:45 AM
Apparently not my last post. A few more tidbits. You said you wanted a filter to keep swarf out of the coolant tank. I think that is where you want the swarf to go. We used filters between the pump and nozzle. Keeps grit off the glass, fixture,and machine parts. Usually only on very tough dig scratch specs. Leica doesn't like it when you send them scratched parts. Like I said though, they are problematic pita and usually not necessary. You want to rinse the machine out before breaks, lunch and at the end of the day. Rinse it all down and into the coolant tank. Last time I checked glass is not water soluble :) gravity is your friend here. It will settle quick and how. I am not a material scientist so I can't tell you why this is but that stuff will harden like cement in your machine if you let it settle and dry out. Also, line the coolant tank with a plastic bag. Heavy duty so it doesn't get sucked up into the pump which you don't want feeding of the bottom anyway. Then when your job is done, drain the tank, lift the bag out and toss it. Wham bam.

In the previous posts I used the terms coolant and water interchangeably which might be confusing. As I said, fresh water will work fine. Company I worked for drilled millions of holes in glass with double sided, core drill tables and only used fresh water. Now if I was going to hog 1/4" off each side of a piece of 2" thick boro on a blanchard coolant additive is probably a lot more important. I think you will find that water/coolant placement and pressure is more important than the mix on your job.

If your using a air-hockey style vac chuck and you can't hold the part try routing some open space in the interior to increase surface area. Leave some standoffs otherwise a 3mm thk part will get sucked down in the middle and cause dimensional problems on tight specs. Your part size is right about at the limit for the that style of chuck. Use that covering I was talking about. Razor blade out the routed area. Leave the standoffs and perimeter covered. Ok, I'm done talking to myself.

puti_1104@yahoo
12-13-2007, 09:13 PM
Hi JP3, I really love read your info..I am new and really focus in this area, need to study more..later there will be alot of question that i need to ask you..

puti_1104@yahoo
02-28-2008, 05:49 AM
I machine the glass by using internal grinding wheel rpm of 30k by using high speed spindle attached to CNC machine sabre rpm of 8000.the very slow of feed rate 0.5 mm/minutes applied.full flood coolant.150grit size internal grind wheel hav been used.

There are chipping at the side of the pocket, is there any clarification of that?
there are other way to avoid that?a lot of question still make me confuse, I have target to have the very best surface finish of the glass machining.
The expert please help me, tq

jp3
02-28-2008, 11:50 AM
Dude, expert is a strong word. I did this for a long time and learned a lot but definitely not an expert. I should also mention that I am sure improvements have been made in processing in the last ten years that I am not aware of but since your stuck with me for the meantime I am happy to impart any useful knowledge I have to you. Can you give me some background information on your part:
1)type of glass- soda-lime, boro, float, cast
2)post process size and thk
3) From the photo the slot looks blind. Plunging in or from the edge?
4)as far as the surface finish I quote Henry Thoreau (or was it Schroedinger? :) - Quantify,Quantify!
What is the "very best surface finish"? Sounds like something an inside sales engineer would say (sales engineer = oxymoron) ha ha. Can you put a finer point on that? It makes a world of difference in how the part is processed.
5) tooling: manufacturer, tool holder/taper/precision, vacuum chuck or clamps.
A few observations based on the info you have already given:
How about the rotation of the tool with respect to the direction of feed? Looks like your feeding in with one pass. If so then you are "climb milling" on one side. I can only see one side and the end of the slot. The chipping at the end of the slot possibly from dwelling too long. Try vectoring back out and up in a continuous movement at the end of pocket. You didn't mention smoke and fire and I don't see any evidence of burning so I assume your getting some liquid into the grind. Are you talking about chips into the face or actually on the edge. Without knowing S.F. numbers I might suggest a rough pass with a 80/120grit plated tool with relief. Then come in with a 180 or 220 grit plated or bonded tool and "conventional mill" the final dimension. The picture of the tool looks right although it looks more aggressive than a 150 grit. Also since the slot is blind is the tool plated on the bottom. Not all of them are. The diamond on that tool is a little sparse as well. The quality of tooling used to vary tremendously. BTW, just so were both talking the same language: chips into the face and surface finish of the grind are two different specifications. I'm not exactly sure which one your referring to by surface finish. If it really is surface finish that your looking for you might have to go with a final pass of a small bonded tool.
Also 20mm/min is extremely slow. Sometimes the concept of loading the machine/tool can be useful. At that speed your almost dwelling. Is the precision of your tool/spindle up to that? More load on the machine might provide a more stable grind. Resonance might be rearing its ugly head here. You have to search around for the sweet spot. As far as the high speed spindle goes I feel like I'm beating a dead (spherical) horse here. Yes I understand the theory. Problem is you put theory in one hand and empirical evidence in the other and see which one makes you more money. Wow! 30k spindle attached to a 8k spindle. How does that even work? Sounds like a violation of kinetic coupling theory. Is my old boss working for you now? The guy never machined a part yet somehow knew that every problem could be solved with a higher speed spindle. Anyway, what rpm are you using? Have you tried varying the rpm? What is the runout on the tool? Give me some more info and I'll help if I can.
-j

puti_1104@yahoo
02-29-2008, 03:33 AM
hi,
1) i am using normal soda-lime glass, no heat treatment
2) 80mmx25mmx40mm
3) tool is coming from the edge
4) i am looking for mirror surfacce finish which is the lowest RA value.
5) manufacturer- taiwan, tool holder-high speed sindle/taper-no taper/precision- not sure, rubber side based - clamps. yes, only one pass.
i am doing almost like face milling process. i vary the rpm, 30krpm and 20k rpm. the noisy sound exist during machining. surface finish i means the finishing of machining surface. here i attach a few more picture.
:)
tq

A few observations based on the info you have already given:
How about the rotation of the tool with respect to the direction of feed? Looks like your feeding in with one pass. If so then you are "climb milling" on one side. I can only see one side and the end of the slot. The chipping at the end of the slot possibly from dwelling too long. Try vectoring back out and up in a continuous movement at the end of pocket. You didn't mention smoke and fire and I don't see any evidence of burning so I assume your getting some liquid into the grind. Are you talking about chips into the face or actually on the edge. Without knowing S.F. numbers I might suggest a rough pass with a 80/120grit plated tool with relief. Then come in with a 180 or 220 grit plated or bonded tool and "conventional mill" the final dimension. The picture of the tool looks right although it looks more aggressive than a 150 grit. Also since the slot is blind is the tool plated on the bottom. Not all of them are. The diamond on that tool is a little sparse as well. The quality of tooling used to vary tremendously. BTW, just so were both talking the same language: chips into the face and surface finish of the grind are two different specifications. I'm not exactly sure which one your referring to by surface finish. If it really is surface finish that your looking for you might have to go with a final pass of a small bonded tool.
Also 20mm/min is extremely slow. Sometimes the concept of loading the machine/tool can be useful. At that speed your almost dwelling. Is the precision of your tool/spindle up to that? More load on the machine might provide a more stable grind. Resonance might be rearing its ugly head here. You have to search around for the sweet spot. As far as the high speed spindle goes I feel like I'm beating a dead (spherical) horse here. Yes I understand the theory. Problem is you put theory in one hand and empirical evidence in the other and see which one makes you more money. Wow! 30k spindle attached to a 8k spindle. How does that even work? Sounds like a violation of kinetic coupling theory. Is my old boss working for you now? The guy never machined a part yet somehow knew that every problem could be solved with a higher speed spindle. Anyway, what rpm are you using? Have you tried varying the rpm? What is the runout on the tool? Give me some more info and I'll help if I can.
-j

jp3
03-01-2008, 03:57 AM
Greetings tq. Looks like we might be converging on a real time conversation here. I read your post and studied the pics. I think I am starting to get a much better idea of what your trying to do. The bad news is you have been given a very challenging problem. The good news is you have been given a very challenging problem :)
With regards to the close up pic of the route: If you look at the very end of the slot the lower-right corner of the radius show a small continuous line of chips. That is inherent to the grind process from a 150grit grind in a good setup.Think of it as a cross section of the surface finish. In the photo you will also see "scallop" chips into the face (float side of part ) These look like they are about 5x times the distance into the face compared to the normal chipping. Those scallop chips are impact chips and not part of the ideal grind process. If you look closely at the scallops their shape directs you to the point of impact which appears to be coming from your tool unless your set up is moving. That is why I asked about your tool/spindle/toolholder precision. At the rpm your running at the slightest micro bump is going to cause those impact chips. We used precision er collets/cat 40 toolholder and then you still had to usually remount/rotate or try a few tools to get the absolute minimal runout. As far as the giant chips in the lower part of the picture and upper right those look sort of like large impact chips but its hard to tell from the photo. They could be from heat/impact. The bad vibes could be coming from your table. I've run a Sabre500 and I know its a good machine but your the judge of your machine's condition. Ok so much about chipping/precision for now. On to the REAL problem here. How to get a mirror like finish in the bottom of a slot.
I thought you were talking about surface finish but you mentioned chips too so I wanted to clarify. Also are we talking about just the bottom of the slot or the sides of the grind also with respect to surface finish? In a previous post I was a little negative on coolant additive. This is one case where you might need it. If your already using it you could bump up the concentration. Another issue is coolant pressure and placement. I see you have some loc line with what looks like maybe a 3/8 or 1/4 nozzle. Pump capable of higher pressure? Your going to need to get that coolant right down into the grind action. Is that just one line? I can't see if there is another one behind the spindle. I have used as many as 4 but 2 is a minimum. Also try switching to a fan tip or at least a smaller nozzle to increase pressure. You will need good strong coolant pressure in a well defined stream. On a route I would use a fan tip horizontally positioned aimed right at the bottom of the tool as close to the tool as practical. Edge grinding I used to use the tip positioned vertically right on the edge
of the tool on the side rotating away from the direction of the stream. On a edge route I would use two nozzles: one horizontal and one vertical. In a one pass route your effectively grinding on both sides and the bottom so I would use a third fan tip on the edge 180 deg from the other for a total of three. I will try to draw a picture and post it . In your pic I see a some scratching and possibly a little glazing on the finish of the grind. I should have mentioned earlier but the 150 grit is never going to get you a mirror finish. I don't like the way that finish looks for a 150 grit but even an ideal 150grit grind is going to be too rough. On the other hand, any tool/process that is going to give you a mirror finish is never going to grind the bulk of the material out of that route so a multiple process is almost guaranteed.
If it was me I would first try to get a clean grind on that slot to make sure my machine, tool chain and coolant placement were good to go. That way you can eliminate a few fundamental variables. We need to flesh out what your looking for as a surface finish. Mirror finish/ low RA number is a good start but need to go a little further. Maybe define the range of RA that is OK for your app. At some point your going to move from grinding to quasi-polishing(my terminology) to polishing based on the RA number. If the latter is the case then your going to be trailblazing because your probably going to have to make a custom polish tool. Polishing the slot, if thats even possible, will require a much better surface finish than you have now anyway so your still going to need to solve the grind issues. Where there’s a will, there’s a way. In the meantime let me get that coolant drawing for you.
-j

puti_1104@yahoo
03-20-2008, 11:39 PM
Hi JP3,

Here are some question that need some clarification because i am not quite sure of what do you mean.

1.i am no sure what do you mean by 'try vectoring back out and up in a continuos movement at the end pocket'. could you please give me an example or sketch of that method

2.How dwelling can lead to chipping condision coz as far as i concern, dwelling is regarding to time of short rest of drilling process.

3. Do you mean 'fan tip' is refer to a very high stream of fluid(air/liquid)?

4.There are noisy sound during the mechining process, is ther any reason?or how to eliminate that..

5.For ductile mode machining process, i need some information on how to identify the citical depth of cut.

6. From my point of view, the method that i use is face milling. i am not sure about climb milling that you mentioned before.How face milling can be climb milling?

Currently, i still run the process, my boss is pushing me to have the best result on this work.Regarding to the coolant pressure, i still have no idea on how to increase the pressure so i still using the full flood coolant method.



BTW, you give great information regarding to this. You are absolutely right that i am not going to have a mirror surface finish by only one pass machining.


TQVM

jp3
04-09-2008, 01:39 AM
Sorry it took me so long to reply. I had some emergency field work to take care of. I just got schooled in a few engineering axioms: 1)any system that fails to take into account the user of the system is doomed to fail and 2) if the system you designed is non-deterministic it is going to suck to be you :) but those are posts for another thread.
Okay, back to the topic. I am going to try and attach a sketch to this post. I'm not sure if this will be legible as I had to jump thru a few hoops to get this in a file format I could post. The last version of autocad I owned was Version 10 with winders 3.1. Now I only use macOS and ubuntu linux and I can't seem to find a good drafting program for either of these. Or at least one that does not require an IPO to finance.


-j

jp3
04-09-2008, 09:49 PM
From your above questions:

1)What I mean by that is basically don't hang around in the slot with a unloaded tool. It's like grinding an O.D. on a lathe with two passes. After you finish the first pass you wouldn't want to wheel the carriage back without backing the tool away from the part first. Since at this point the tool is the same diameter as the slot the tool will "bang" the edge of the route causing chips. Try to keep a load on the tool until you clear the part. I used to tweek my programs by literally hard coding a small section of the tool path.

2) This is related to the above question. Your definition of dwelling is the same as mine except that you can generalize that to any process and not just drilling. In this case I was referring to the fact that you are feeding so slow that the tool is essentially unloaded and grinding the same spot. Unless your system is very rigid and precise the tool will behave differently loaded verses unloaded. And by different I mean you will ding the sides of the route with the unloaded tool. Your mileage may vary.

3) yes i found the fan tip made it easy to get a thin sheet of coolant at a higher pressure than you can get from the round orifice tips. The orifice on the fan tips is just a small slit. Ever place your thumb on the end of a garden hose to increase pressure? Maybe you can pinch the coolant line or something. Improvise. I seem to remember once taking a lighter to a round tip and heating it until it was soft and flattening the tip when I couldn't find a fan tip.

4) Well grinding is a noisy process. I have the hearing loss to prove that :( but I'll trust your judgment that it doesn't sound right. As far as that spindle speeder that you have in there I really don't know much about them but the few that I researched on the intertubes looked cheap and possibly not suitable for grinding. Is that one of those with the gears or is that an air turbine? Can you describe the noise ?

5)This would be one of the areas that has seen significant development since I left. I never had a surface finish requirement on the vert mills like you do. We achieved a quasi ductile mode (50%??) on other machine processes but polishing was usually necessary anyway. Very high feed rate, high SFM, high pressure coolant and very fine resin bond tool and depth of cut in the tens of microns. I looked around and found a remarkable number of research papers on the subject, many of them from your neck of the woods (Singapore Uni) so there is obviously a large amount of interest in the subject. The text "Microfabrication and Nanomanufacturing" by Mark J. Jackson looks like an excellent resource. Pertinent sections of the text are available via amazon.com preview. I suggest you check it out. He provides a model for ductile mode machining. No derivation shown though it appears to be for a single point tool on an OD lathe process. He also used a cnc'd Moore jig borer for grinding which probably has your mill beat by at least an order of magnitude on several of the critical specs. Maybe if you can relax the tolerance and form constraints you might still be able to hit the surface finish. We used an entirely different process for making I.C. substrates. Also, as you might have noticed the rough grit plated tools provide quite a beating to the glass (maybe the source of the noise?). I've never measured the fracture depth but it must be substantial which is why I suggested a intermediate pass to clean that up.
Jackson used a tool with a slight cone shape on the bottom and then looked for the ductile streak zone with a microscope to determine the critical depth which in his case turned out to be approx 10um. Another idea might be to face a piece of glass with a tool while varying the depth of cut at the smallest increment and mapping this out on paper so you can relate the depth of cut to a position on the glass when you take it to inspection to observe.

6) The climb/conventional mill idea refers to the rotation of the tool with respect to the direction of feed. This was in reference to the chipping on the walls of the route. I'm not sure how that would apply to the bottom of the tool (face?). I'm going to have to let that one soak around in the brain for a while. My experience was conventional mill produced less chip and chatter. Hopefully I drew that correctly above. I always have to think about it ten times before I'm sure I have it right. Kind of like using the "right hand rule" with vectors. I think your on the right track. Look for a resin bonded tool if you can find one that small.

-j

anonymality
08-22-2011, 08:27 PM
Hole example;

10mm thick glass.
19mm dia. blind hole 9mm deep (1mm from going though).

1- I use 10mm metal bonded diamond core drill (Mole Moreschi).
@5000rpm - 1500mm/min and with freshwater flood.
I drill 3mm holes on the side of the tool to help the water to go inside.

2- Start ramping down at final diameter 0.05mm stepdown.

3- 1/2 feed when you reach 2mm thick floor to prevent bullethole-like
breaking of hole bottom.

4- make pass @ final depth.

There will be some microscopic chipping but nothing major. You can still reduce entry feed for the first 1mm or so to reduce chipping.

The advantage of metal bonded core drills is that they "refresh" themselves while using them because the glass dust sandblasts the metal bonding revealing fresh diamonds to grind trough glass.

Be carefull when using thru coolant tooling because the pressure might break the bottom of the hole.

I make slots the same way. and choosing various drill diameters according to your hole/slot dimensoins may do a big difference in the time needed to do the task.

CAUTION! if your want THROUGH holes/slots you have to finish them from the other side of the glass or you'll end up with bullet-holes.

Edit; Don't forget to lead out towards center of hole/slot or you'll make chips while getting out if your tool still touches the machined wall.

anonymality
08-24-2011, 08:08 AM
The advantage of metal bonded core drills is that they "refresh" themselves while using them because the glass dust sandblasts the metal bonding revealing fresh diamonds to grind trough glass.

Excuse me for QUOTING myself but here's a VERY inportant note;
Some brand new metal bonded diamond tooliing have too much bonding on their surface and may cause too much friction and therefore chipping the glass.

What you'll need is some specially made stone to "refresh" your tool. (probably available where you buy your diamond tooling).

Just make the tool rotate @ +/- 500 rpm and hand grind the DIAMOND surface of the tool with the stone and freshwater.