[john@tlt]

I just upgraded to V26 of BobCAD. Our router spindle does not have thrust bearings so the boss is concerned about our plunging. I cut 24 12.5dia. circles from a 48x96 sheet of plywood daily and am trying to find a way to bypass multiple plunges. If i can have just 1 plunge on the edge of the sheet and create adjoining toolpaths, it will cause a lot less strain on the spindle in the long run. Anyone know how to link cuts together without plunging into every part?

[mmoe]

You could do it, but it will take some extra drawing. Ironically, something like V20 would probably do it better because of the way the toolpaths were generated back then. The newer software makes difficult tasks easier, while the older versions were such that you would basically draw the toolpath and then generate the code from it. Essentially, you would offset lines around the circle, then you could connect the offset circle lines with joining lines and run the tool along all of the lines in one long motion, which is what I think you are after.

You could probably still do that today in V26, but it would require that you offset the geometry and trim the lines to create on long line running the path you want the tool to follow (including the tool offset if you don't do this in the controller). Once you have your long path created, you could then do a 2d profile of the line, without using an offset and it should just follow the path. It may get confused where lines crisscross, which I don't think is avoidable, so you may have to select each line in sequence one by one rather than doing the shift/click selection. I would bet it's possible, but definitely not something the software was optimized for. If I have time, I'll see if I can get it to work that way.

[jrmach]

mmoe,problem with that,contours do not seem to work from a circle to a line to a circle.The circle would need to have an actual break point/gap to work.The only way I think may work,is at the intersections,actually have the geometry vary in Z height so your geometry is one continuous entity.Kind a like an overpass/underpass.This could be very minimal,just enough so the actual lines and arcs don't touchThen you would use 3D engrave.
Think of it as a spiral,technically,connected to a line,then to a spiral.
The idea,not letting the geometry physically touch when criss-crossing.
Do-able,but some work.
How about drilling entry holes for where you will plunge ?

[john@tlt]

I have been plunging at an angle to cutdown on stress. We have an airdrill mounted for drilling but sadly I am still new to the CNC Programming game so I haven't yet worked it into a program. I have tried to "nest" the parts onto a stock but they will only line up 3 by 7. The way I have them currently positioned, I am able to add 3 more parts by offsetting them up 6 inches on every other row. If I can set all toolpaths/gaps to the correct distances and add an extra toolpath, would plunge roughing around the parts be an option?

[jrmach]

Here is something along the lines that I am talking about.This over/under could be as minimal as a .001.Just so the geometry does not touch.

[john@tlt]

Sadly, bobcad now tells me that there is no possible way of obtaining a "Common Line" cut on their software. Any software that will still do this on the market these days? Preferrably Freeware....

[jrmach]

I am not following you.

[bhurts]

What kind of spindle are you using. If this is a business and the spindle can't plunge or ramp into plywood that's pretty crazy.

Ben

[mmoe]

Here's a way you can do it. I basically divided up the circles into sections, created paths to connect the sections, and then when there was going to be an overlap I moved the overlapping paths to a new layer. Each layer then gets processed as a separate toolpath. At the end of each toolpath, the tool moves up to rapid position, then back down to cutting position, but there is technically no material there, so it's not really plunging. If you set up your rapid right, you should only have a short delay between each toolpath, so not really a big deal. Where the sections are for each circle that connect to a straight line between circles, I added a fillet/radius. Because of that, when you do the opposite part of the circle, you need to overlap the toolpath so there aren't any uncut portions (look very closely at the drawing).

I didn't really draw the circles to any scale other than close to 12.5 inches (I work in metric and was being lazy). The concept would be the same though. Start with your circles. Offset the circles by half the diameter of your cutter to the outside of the circles. Trim and connect circles into toolpaths on separate layers. Generate toolpaths. Verify in simulation.

Hope that helps.
-Mike

Here's a simulation of my machine cutting the file. It's an .exe, but it's not a virus no matter what your browser might think. You don't need to install it to simulate the cut, just run the .exe and you'll see how it looks in action. No plunging anywhere that there is material and not a whole lot of wasted time either.

https://files.secureserver.net/0srvqDD8b5Nq31

[The Engine Guy]

From reading all the above posts I too am amazed that a machine exists that won`t ramp into plywood and then do a ramping contour ? ? ?

However, may I respectfully suggest that instead of spending huge amounts of your own and others time on this that you just get on with getting the drilling machine working, that should be your priority I would think

Regards
Rob
:rainfro: :rainfro: : rainfro:

[mmoe]

If the drill function was working, a person could draw a set of points at the start position of each toolpath and drill a clearance hole for the bit to plunge into. That would also be a good solution until a router spindle with thrust bearings is installed (which is really the best solution).

I'm guessing the drill is offset from the router, so you'll need to use work coordinates for each tool to make that work. I use the same thing on my multihead router, so if you need help getting your post processor configured to work with the drill, let me know. I actually have 2 routers and 2 drills on my machine for a total of 4 different heads that are really working in 4 different coordinate systems if you don't compensate for their location. I have mine set up so that if I select tool number 1, G54 workspace is called out in the post processor along with an M31 command to select head number one as active. Tool number 2 calls out G55 and M32, tool number 3 calls out G56 along with M33 and tool number 4 calls out G57 along with M34. Each of those are then offset in X and Y in the controller so that they all align onto the same coordinate system when the program is running, so it works out like having a single head with a toolchanger. The modification to the post processor to automate this function is pretty simple. My guess is that all you need for the drill to operate is a post processor such as this which calls out both the machine code to select the head and the workspace code to align the heads.

If this is a Mach 3 controller on the machine, I can also suggest how to configure the controller so that a Bobcad post processor is easiest to provide.

[mmoe]

From reading all the above posts I too am amazed that a machine exists that won`t ramp into plywood and then do a ramping contour ? ? ?

However, may I respectfully suggest that instead of spending huge amounts of your own and others time on this that you just get on with getting the drilling machine working, that should be your priority I would think

Regards
Rob
:rainfro: :rainfro: : rainfro:

I think it's a handheld router that has been installed into a CNC router, such as a Dewalt or Porter Cable. Those do have what are mostly radial bearings that can take some degree of thrust, but they weren't really designed for any more thrust force than a person can manually apply by pushing down on it without the aid of any kind of mechanical leverage. I do think that in reality, a feed rate of perhaps 50 ipm or 1000mm/min would be perfectly acceptable for that kind of router and would last years that way.

[jrmach]

I think a hand held drill,a tape measure,a pencil and a tiny bit of layout work,and you can drill your starting points quick as snot.

[john@tlt]

This is actually a very nice spindle 16hp If my memory is correct. It can plunge but the owners feel that it is pushing its limits plunging more than once a sheet. I have it ramping in and doing what it should be doing but when they purchased the machine, to upgrade the spindle with the company that reworked out table would cost approx 25,000$. So to help them rest easy is why I am looking for a way to bypass plunging on every single part. Thanks m moe. I will try that out.

[mmoe]

This is actually a very nice spindle 16hp If my memory is correct. It can plunge but the owners feel that it is pushing its limits plunging more than once a sheet. I have it ramping in and doing what it should be doing but when they purchased the machine, to upgrade the spindle with the company that reworked out table would cost approx 25,000$. So to help them rest easy is why I am looking for a way to bypass plunging on every single part. Thanks m moe. I will try that out.

I'll apologize in advance for this long reply, but I hope it helps. If you want, you can let me know what kind of machine and what kind of spindle just to be 100% sure, but I doubt there is any way I'm off on this from what you describe.

If the spindle cost more than, say, $2000, it should be able to plunge all day, every day without even noticing that it's doing so. If the machine has a 16hp head, which is massive by even the most industrial CNC router standards, it is an industrial machine and meant to run 24/7. In fact, you can probably plunge with dry tooling in aluminum all day, every day if you want and do so for years without problems. As you can see from my simulation in an earlier post, I have a pair of approximately 7-10hp heads (not specified on the heads, but have 4.5kw VFDs), and I am currently running a program that plunges 4626 times for each head (both heads cutting simultaneously, so 9252 times in total per cycle), all inside of 3 hours per cycle. I've owned and been using industrial CNC routers for around 15 years and I have never had any concern about plunging. Each head on my current machine runs about $10k to replace and my previous machine had a pair of heads that ran about $15k each, so I know what it's like to worry about having to replace them. To be perfectly straight though, I don't worry about the heads for plunging at all and my experience has been that it just doesn't wear them out. What generally wears them out is poor maintenance, running them near max RPMs (I prefer to stick to closer to 15k on heads that are rated for 18k), and not warming them up a bit before you crank them up to high RPMs (a 3500 rpm warm up for about 3 minutes prior to cutting is what I do to bring the bearings up to operating temp before going high speed). Even if you do those things wrong, an industrial spindle will last years and can be rebuilt for a fraction of the full cost of replacement. Personally, in 15 years I've not had to replace one at all, though I'm a smaller shop and run them at probably only 10% of their capacity. I'll run them to death for a couple of weeks on a big job (such as now), then have a lull for a few weeks where I only do a one or two hour job every couple days until I get the next big job.

The biggest concern I have about plunging, and what I know is wearing out more than anything, is the Z axis lead screw. While an industrial machine typically has a design that counterbalances the weight of the head with air assisted lift, it's rarely perfect and there is some degree of wear that occurs to the lead screw during Z motions. This is especially true of a machine like mine where the Z axis weights somewhere around 1500 lbs and moves at rates up to 400 in/min (will soon be 800 in/min). However, this still takes years to become an issue, and since I charge $100-$150 per hour for machine time, I can afford to put a $2000 lead screw in the Z axis every 10 years. If someone came to me with a job cutting circles out of 10,000 4x8 sheets, I would plunge for every one of them without even the slightest concern about it. As I said, I'm currently doing a job where in a 4x8 sheet, I'd plunge with a singe head for 9252 times (the 4626 was in a 4x4 sheet). Between the two heads, I plunge double that per 4x8 sheet. Over the entire job of 12 sheets, the machine will plunge a single head 111,024 times and both heads totaling 222,048 times. The machine still works the same today as it did before the job even began and it's nearly finished. For an industrial router, that's really nothing and just business as usual. For 10,000 sheets of circles, you'd only plunge 240,000 times, just to put that into perspective. You could machine nearly 10,000 sheets of circles to equal the plunging I've done in 12 sheets of the parts I'm making now. Again, my feeling is that the real wear is occurring on the Z axis lead screw, but if I can plunge a 1500lb Z axis nearly a quarter of a million times in about 2 weeks worth of work with no perceptible wear, you should have no problems plunging 240,000 times in what would be about 6 months worth of work doing 10,000 sheets of circles (figuring about 6 minutes per sheet from cycle start to cycle start).

It should also be remembered that there is one plunge per part in your case, so that would be 240,000 circles cut in a 6 month period (if you were doing 8 hour day production). If you were making even 50 cents on each circle, that's $120,000 worth of profit, and I seriously doubt that the spindle would have even had a dent in it's lifespan by then. You really just have to let the machine make money, and factor that some of that money will eventually go into repairs so you can keep making money. I once calculated that a new machine of the $150k-$250k type can most likely produce around $2 million in product before it becomes what a manufacturer would consider unreliable from a maintenance perspective. At that point, it can still function well for a shop such as mine for decades before it's worn out and needs a complete overhaul.

Then there's the comparison to the alternative to plunging. The main point of a CNC router is speed and production, so don't take the speed out of it if you don't have to. By not plunging, you would increase the time it takes to produce the parts by 6% in total run time. You also are increasing the time the head is engaged with material to create the same number of parts. In my experience, that's hurting in two ways. First, you're wearing your cutters out faster, probably by perhaps 10%. This is really going to add up over the long haul more than you think. It may make a $500 difference in a six month period of time if you're making parts on a production level. Sound far fetched to spend $5k on tooling? In my current 2 week job, I'll have worn out $300 worth of bits, so if I continued to cut the same job for 6 months, I'd use about $3600 worth of tools and would loose $360 if I wear them out 10% faster. Those are inexpensive bits because they are smaller (about $25 each). If you use a 3/8" compression bit with a 3/4" LOC, you'll pay three times that much for each bit (and loose 2x to 3x as much, or around $500-$1000 to premature wear).

In addition to wearing the tool more than you have to, you are also wearing the heads more than you have to. In my estimation, based on my experience and the experiences of other CNC router owners I know, these heads simply wear out from time spent turning. Nothing more and nothing less. They wear out a little faster if they run hotter, which is why I like to run them a little less than full speed, and they wear out a little slower if they run cooler. Either way, they have a life span that relates mostly to the bearing life. If you take 6% longer to cut a sheet of parts (this is the actual simulation difference between plunging and not, but I think it would be greater in real-world conditions), and you spend most of that extra 6% of the time engaged in material, there is no doubt in my mind that your spindle will produce 6% fewer parts in it's life vs. a spindle that has spent less time turning per sheet and less time engaged in material per sheet.

Then there is the practical aspect of how well will the parts hold down and will you damage the bit itself. The simulation I showed is not real-world. It looks like it works great on the screen, and in theory is useful. In the real world, you run the risk of the fall off vibrating enough to break or damage the bit. You also have reduced the vacuum level of the table significantly because every additional inch of cut is additional vacuum leak through the MDF wasteboard (assuming you have a vacuum table). That only enhances the chances that the fall-off vibrates loose and damages the bit. If you plunge, the likelihood that the parts hold properly and nothing unpredictable happens is far greater. You'll produce an extra sheet or two of parts in the same 8 hour day and you'll spend 30 minutes less time programming before you start cutting the first piece. If you have an industrial router head, there really is no advantage I can think of to avoiding plunges. These machines were designed to do this day in and day out for thousands of hours of operation.

If your machine is not industrial, there would be reason for work arounds, but I just can't picture a 16hp head on anything that doesn't weigh several tons (the head itself would have to weigh 200-300 lbs). I'd recommend that you do some research and present a well reasoned proposal to your boss regarding how things are programmed.

Also, as I offered before, I can probably help you get your drill going. From the sounds of it, you likely have a piggy back drill if the head is that big. That's exactly what I run, so I can probably help you get it going.

[john@tlt]

It's a G. Columbo 16hp spindle on a Fanuc 18MA controller. The company that we purchased the router from had told us that due to lack of thrust bearings, plunging was a little tougher on the spindle so I've just gone at an angle which seems to cut down on the movement of the parts anyway. The router is $240,000 new from the company that resized the table but we purchased this from auction for 30k. The router initially came with screw extractors from being used on airplane siding but after having those removed, the air drill installed and the table resized we may have 45k in it. I really appreciate your help putting it into cost perspective. Where we have been paying about 1.40$ per seat already cut to size x 18k a month or so, I now am able to cut 28 on a 9$ piece of particle board. As for our other seats and such, the profits are similar or better. So that being said, I'm sure that with the amount of profit we stand to bring in will be a valid point if this Common Line issue comes up again. If you are interested in helping me with the AirDrill, I would appreciate it greatly. All I have been told was that the code for operation is M51 but my post processor is currently a Generic post with simple G90, G54 and cuts. I have yet to get involved deep enough to use the M-Codes. Thanks for the help!

[mmoe]

That's a pretty heavy duty router and I don't think a piece of particle board will make a hill of beans difference to it. For all practical purposes, plunge cutting particle board with a center cutting router won't be much different than cutting air to a spindle like that.

Is the Columbo a toolchanger or a single tool spindle? Is there an M code for the main spindle start as well? Usually, multihead routers have an M code assigned to each head. For example, for head number 1 on my machine I use:

M31
M3 S15000

while for head number 2 I use:

M32
M3 S15000


My old machine could have the M code on the same line as the M3 command and went like this for head 1:

M03 M13 S15000

while head two for that machine went like this:

M03 M23 S15000

In the case of both machines, turning the spindle off basically cancelled out the spindle M code. So if you use M5 or M05 with either of them, you have to the restate the head you want to turn on the next time you have a spindle start command. M3 or M03 with an S value does nothing without M13, M23, or M31, M32; etc. It would be good if you can show me a sample program which includes the spindle start for the main spindle.

The other thing you will need to figure out is if M51 also compensates for the shift in coordinate systems, assuming that the main spindle and the drill are not centered on each other (such as a rotating turret). Also, do you use tool length compensation or do you just set up your Z0 based on the tool after you install it?

What is your monthly output of these parts and do they change much or are you running the same couple styles of part over and over?

[john@tlt]

The columbo is a single tool spindle. I have been setting up my Z0 after each change since tool changes are so rare. I use M03 S16000 to start the spindle currently. The M51 compensation is unknown currently, I have the handbooks from this but have yet to find anything about it. Our monthly output changes currently. I have been testing out a few new products that we have been ordering for the past few years. I have the spoil boards and programs safely stored for each job but have changed to custom table tops today. I have found that the company has been ordering a 60inch diameter table top with a simple 1/4x1/4 deep channel cut 2 inches in all the way around for about 95$ a piece. I can cut them for about 10$ in 5 minutes. I guess that the airdrill will be my new priority. If I can get the air drill working, it will cut down on a lot of extra drill holes and center cutouts. Would you recommend running a small program while using the M51 code to see or should I continue reading/contact the company about the coordinate system compensation?

[mmoe]

If you just use M03 to start the main spindle, my guess is that M51 is the only code needed to start the drill. Drills often don't use an "S" code since they are not usually powered by a variable frequency drive. Basically, the drill will run at the name plate RPMs, probably around 3500 RPMs. It's just either on or off.

The drill is probably on a pneumatic assembly that lowers it to working position? If so, M51 likely lowers the head and turns it on. It's about 50/50 whether or not the controller shifts the coordinate system as well as I think it's probably capable of doing so and it would have been more of a setup decision by the machine manufacturer. If you know how to do manual data entry, try just typing in M51 and see what happens. Obviously, when trying things that you don't know what the results will be, have a hand ready on the E-stop! If it does as I suspect, the head will lower and the spindle will turn on. Do this with the Z axis at it's highest point just to be on the safe side.

Note the X,Y,Z coordinates before you enter M51, and then note what they are after you enter M51. If they stay the same, one of two things is likely. Either the coordinates displayed are the machine coordinates, not the current work coordinates (unlikely in my opinion, but I'm not that familiar with Fanucs in practice), or the coordinates are the work coordinates and have not changed with the M51. If the coordinates change, you know they are the work coordinates and that M51 automatically offsets the coordinates for the drill in X and Y. If the coordinates are the same, but you are able to determine that they are work coordinates rather than machine coordinates (more likely work coordinates), then you will need to use a separate G code command to shift the work coordinates.

Some controllers have provisions for offsetting the coordinate system for mechanical design reasons without using one of your work coordinate (G54, G55, G56, etc.). If the coordinates change, that could be the case and would be able to be determined by noting what work coordinate you are in. If you started in G54 (standard default work coordinate designation), and it remains in G54 but the coordinates change, this change has been done in a configuration setting rather than through G code and no additional G code would be needed. In some cases, the machine may even move to align the drill with the previous coordinates of the router automatically, so don't be surprised if the machine starts moving, but don't let it dive into the table either. If the G54 changes to something else, you'll have to let me know what that is, but I think it will likely not happen. If the head turns on and lowers with M51 and automatically aligns the coordinate system with the router spindle, then you will either have a line where you use "M51 T2" where you use the tool length offset in T2 to compensate for the difference between the main spindle and the drill. In that case, you would probably also have to start using T1 offset for the router, which really won't be a big deal once you learn it and as you've pointed out won't need to be done very often if you don't change the tool. If the head lowers and starts, but the coordinate system doesn't seem to compensate automatically, I would recommend you would use "M51 G55", which would use a separate work coordinate system to compensate for X and Y, but then you can also compensate for the tool length to align it with the main spindle with the Z offset in G55. In that case, there is no need to use the tool length offset since you essentially are doing so by configuring the Z offset in the G54 and G55. If you find tool length offsets to be difficult and would prefer to use G54 and G55 when the head has already compensated in X and Y automatically, you could just set G55 to an offset of "0" in the X and Y (since it already did it) and use the Z offset as in place of the tool length offset. You would then just configure the Z offset in G54 for the router spindle and G55 for the drill instead of using T offsets.

Hope that's not confusing! You can start by just testing the M51 code and letting me know what the results are and what the readings on the coordinates and G54 came out as. I can narrow the info down after that. The other part of the puzzle will be figuring out how to turn the drill off. I would not be surprised if the code for shutting the drill off is "M50" instead of M5 or M05. Once you get it going, try using M5 or M05 (depending on your controller's preference) first. If that doesn't work, try M50. If neither works, hit the E-stop and let me know the results so we can figure it out. Perhaps the previous owner can also clue you in on the stop command if it's neither of those. I once had a machine that used M50 for the stop command for all spindles and a lot of times M codes are canceled by the first M code of the series. For example, if you had 5 heads, they may be selected by M51, M52, M53, M54 and M55, but all of them may be cancelled by M50. Since M50 is quite similar to M5, it just seems logical if it's not M5.

[lixingwen1987]

I AM GLAD TO TAKE THIS OPPORTUNITY TO INTRODUCE OURSELVES AS ONE OF THE LEADING SUPPLIERS OF Precision Bearings for CNC and Machine tool ,AND YRT bearings WHICH ARE FROM THE REOWNED MAKE OF Wafangdian Tianjiu Bearings Technology Co.,Ltd.,.

WE ARE IN THIS BUSINESS SINCE LAST FIFTEEN YEARS; IN THIS SPAN OF TIME WE HAVE SUPPLIED PRECISION IN ALMOST ALL THE CONTINENTS OF THE WORLD.

OUR BEARINGS WITH COMMON PRECISION ARE MAINLY MIDDLE / LARGE BALL BEARINGS, ROLLER BEARINGS AND SELF-LUBRICATING JOINT BEARINGS. OUR SL BEARINGS ARE FAVORED BY CUSTOMERS. BESIDES, WE DEVELOP HIGH-PRECISION YRT ROTATED BEARINGS, MACHINE TOOL MAINSHAFT BEARINGS AND MOTOR PRECISION BEARINGS. THE PRECISIONS OF OUR BEARINGS HAVE REACHED LEVELS OF P5, SP, P4 AND UP.

FEATURED BY HIGH PRECISION, LOW NOISE, HIGH ROTARY SPEED, HIGH QUALITY AND LONG SERVICE LIFE, OUR PRODUCTS SAVE USERS’ COST AND SHORTEN PURCHASE TERM. WIDELY APPLIED TO COMMON MACHINE TOOLS, CNC MACHINE TOOLS, LARGE / MIDDLE MOTORS, PRECISION ROLLING MILLS, ETC., OUR PRODUCTS FILLED THE DOMESTIC BLANKS AND CAN SUBSTITUTE IMPORTED PRODUCTS.

THIS IS TO INFORM YOU THAT WE HAVE PRECISION BEARINGS AND OTHER GOOD QUALITY BEARINGS AVAILABLE, CAN SUPPLY FOR YOU WITH BEST QUALITY.

PLEASE SEND US YOUR REQUIREMENTS IF YOU HAVE BEARINGS NEED.

WE CAN SUPPLY OUR BEST PRODUCTS FOR YOU.
Wafangdian Tianjiu Bearings Technology Co.,Ltd.
(Wafangdian Heavy Bearings Researching & Manufacturing Co.,Ltd.)
Brand：WZFB
Web: 瓦房店天久轴承科技有限公司（原 瓦房店重型轴承研究制造有限公司）
Tel: 0411-85366785
Fax: 0411-85366785
Mobile:+86-15942617721
E-mail:[email protected]
Q Q : 178702120
Skype: lixingwen1987

Do our best to give customer best service.