FYI On Cat V Flange and BT tool holders the tapered shank is 7:24 and that's on diameter so per side its' 3.5/24 which works out to 8.297 per side angle (ATAN3.5/24), which is greater than the included 15 degree locking angle such that it is self releasing taper. Cheers! Len Dye edit: sorry, should've checked my work instead of going of memory

MasterCaM Rookie I pretty much got it to work with just a couple little issues now. It looks like you will be to do a full simulation possibly too. When you get a chance check out the latest file that is attached. Cheers! Len Dye MASTERCAM HORIZONTAL MILL 1 PART.zip

If you choose tapping, which IMHO is faster and has less tooling costs per hole when compared to thread-milling, you DO NOT want to use a spiral flute tap, they're only good up 2X diameter or less otherwise the flutes will pack up with chips and it will break. Rather you want to us a spiral point tap that pushes the chip in front, thru the hole. A spiral flute tap is the weakest type and a spiral point is the strongest other that form taps. Being the part is steel you would want either the Steam Oxide coating (black) or the TiCn coating and Powered Metal as opposed to HSS, like the OSG VC10 grade. Cheers! Len Dye

I took a look at your file. I typically don't program multiple parts but rather just 1 part for OP1 and 1 part for OP2 and would use "Transform" tool paths for the remaining parts. . Also I won't have all the solids for the tombstone and clamping in the file because it just clutters the screen, slows it down and makes it cumbersome to work with, but that's my personal preference. However the tombstone & fixturing would be included in my simulation thou. If you want to do full simulation on all the parts at the various table positions you may have to do it the way you have it now (all 24 parts) because of the way transform works it might post right but not simulate proper or visa versa, I just don't know transform well enough to tell you that it would work with programming just 1 part using "Fixture Tracking". It is working for the 1st set of parts at B0 but I couldn't get it to post the 2nd set of parts at B90 proper using transform/rotate. It maybe a setting or an is a function of the post?? (see my example program attached) The way I'm talking about your OP1 & OP2 parts for each operation would be at their respective X, Y & Z origins (like the lower left corner in my attached example) Regardless you did not have your tool planes proper in your file. You want to use WCS= Top and Tool Plane & Construction Plane= Front, this is your B "Zero" primary tool plane and is viewed as if you're looking at the part from the spindle for your Part #1 OP1 pocket milling. If you're machining on the right side of the part (B90) you can use the system "Right" tool plane so planes for the tool path would be WCS=Top and Tool Plane & Construction Plane= Right however for machining the left side (B270) of the part you will have to make a tool plane, call it B270, so tool planes in the operation would be WCS= Top and Tool Plane & Construction plane = B270. The same thing for B180, you would need to make a tool plane like B270. I would prefer a separate work offset for each part with an offset for each B-axis position on that part as well. So if your program were to machine the sides of a block also, say at B90 & B270, then there would be a total of 3 work offsets for each part. Being there isn't enough G54-G59 offsets I typically only use G54.1 P1-P48 (or P300 depending on machine) so lets say part #1 is P1 for B0, Part #2 for B0 would be P2 work offset etc and for the set of parts at B90 would be P7-P11 For OP1, Transform/Rectangle toolpaths will output P1-P6 for your 1st tool on parts #1 thru #6 and transform/rotate outputs P7-P12 for the the OP1 parts at B90 but it doesn't kick out the B90 proper for the 1st part at B90, doesn't retract prior to indexing and is using P1 not P7. Maybe you could play with the settings a bit, it might be a function of the post like I said thou??? Also I couldn't get OP2 to post multiple operations proper without having to have a transform for each operation. You would think it would do them in operation order without repeating the 1st part and output a separate offset for each part but I didn't spend much time with it but this worked using a separate transform for each operation. So when using just 1 X, Y Z origin inside of MasterCam (the same lower right corner for B0, B90 and B270) the coordinate output doesn't consider where the part is on the pallet or where center of rotation is, just the coordinates within itself'. There is where my "Fixture Tracking" macro comes into play. Before the part even shows up to the machine you can have all your "Primary" work offsets figured out and written into the CNC program using G10 data setting. The G10 would set X, Y & Z for the P1-P6 set as well as P7-P12 for the 2nd set of parts, and the "Fixture Tracking" macro would calculate all the remaining work offsets for B90 & B270 machining. This way I would only have to program just 1 part for OP1 and 1 part for OP2 not 12 different parts for each tool path as you have it. Also I would only have to make 1 tool plane for the left side (B270) not 72 different tool planes and furthermore I wouldn't need to use an edge finder or whatever to pick 72 different work offsets at the machine either. Certainly once the offsets are read in at the machine you could probe the part for an exact position but you have to remember to re-calculate the offsets with the fixture tracking macro after the primary offset has been reset with the probe so the other offsets are calculated from the new position. However you would need to get Transform to work in conjunction with 1 part and fixture tracking. Otherwise, as you can see, if you programmed all 12 parts and didn't use fixture tracking at the machine there would be a bunch of extra programming to do and would probably be a nightmare to establish 72 different offsets at the machine. I think this is what you should strive for and try to get transform to work with just 1 part while using fixture tracking. In case none of this makes sense then you have to program it the way that you know cause I just don't know how else to explain it. If you have further questions PM me and I'll send you my phone number and try to explain it better. I hope I didn't confuse you because all this can be very confusing but not really complicated once you grasp the concept IMO. Cheers! Len Dye MASTERCAM HORIZONTAL MILL 1 PART.zip

severely also means "rigidly restrained "

yes this is correct, also you don't necessarily need to return the turret back where you left off. On the 1st cycle start the tool will return to where it came from and on the 2nd cycle start it will continue machining where it left off. Cheers! Len Dye

Tool stone is not expensive as Ron said. It's similar to plaster of paris, pink in color not white, it doesn't nut up as quick so it gives you more time to work with it. You can clamp on it with good medium force and it doesn't grow or shrink much and doesn't absorb much coolant. and yes we used to use babbit putty (de-orderized bear shyt) until we found out it had asbestos as its' main ingredient so we now use Deacon Mold-Pac to built damns and moats to contain the tool stone. If you're filling pockets up for support I would start with the putty because tool stone will be much harder to take out when you're done but would provide much better support however with a slight draft as suggested that would help release the tool stone otherwise we just break it apart to get it out. The putty doesn't hold up as well with oil/coolant but in your case it would be underneath so it might not get wet at all. Cheers! Len

Wouldn't you have to check out the document first so there's a local copy, then merge it? We're using Predator PDM for all electronic files now and IMHO it's a steaming pile of poo. Cheers! Len Dye

here you go, It was easy for me to take the time to write it and test it for you. Load the following program into the memory. If you use it a lot you may want register it as a G-Code macro otherwise the command would be G65 P9020 D= number of digits. Start with your number in #100 and it puts the 1st digit into #501, 2nd goes into #502 etc. Be careful thou, its writing to #500's where your probe calibration data may be and you will be recalibrating you probe like I am I tested 9 digits only but I imagine it would fill as many registers that you have. O9020(PARSE OUT NUMBERS) (COMMAND= G65 P9020 D#) (D= NUMBER OF DIGITS TO PARSE) #101=1 #102=0 #106=.001 N1 #100=[#100/10] #102=FIX[#100+#106] #105=[[[#100-#102]*10]+#106] #102=FIX[#105+#106] #100=FIX[#100+#106] #104=[#102+500] #[#104]=[#104-500] N2 #101=[#101+1] IF[#101 GT #7]GOTO99 GOTO1 N99 M99 % cheers! Len Dye

attached is a serial number macro that parses out each number from the value in a macro variable register. Basically it divides the value by 10, rounds it down then subtracts itself from the original number and multiplies it by 10 to parse out the number into a separate register. There is a fudge factor in there that deals with binary round off errors caused by the CNC control. Look at N15 of the macro and you see how it extrapolates the number into #104 then jumps to N#104 to engrave the number at which point instead of engraving a number, you could have it fill the registers as you have it shown here. hope this helps! Cheers! Len Dye Serial Number Macro.zip

Attached are a couple of macros that I use for deep hole drilling. They both feed down inside a pre-drilled hole at 4X the programmed feed (I didn't like rapiding into the hole) Also they both allow you to specify the 1st drill depth prior to pecking because many times you don't need to peck until the drill is in there a ways. In addition both macros allow you to specify the point to retract too within each peck. Many times with long drills you don't want to pull out of the hole all the way to the R plane so I set this to .050 inside the hole. This keeps the drill edge from clipping the part each time it goes in an out of the hole which can cause premature wear on your drill. Furthermore, really long carbide drills will snap off if the drill isn't piloted inside the hole, hence the 2 macros, one with a dead spindle just for this reason. I register them as custom G-code macros G183 & G283. hope this helps Cheers! Len Custom Drilling Macros.zip

That should be #7081 not #7801 for P5 work offset

Our Mori Seiki's have Nikken and the newer ones have Mori's rotary table which are really nice for mill-turn applications because they are direct drive, no gears and no back-lash. Although we don't normally do heavy cutting while mill-turning, someone previously did on one of the Nikken and the table had excessive backlash so the gears had to be replaced. that's my 2¢ Cheers! Len Dye

Here's a "fixture tracking" macro that I use on horizontals in conjunction with MasterCam and explanation thereof. Also attached is a serial number macro for Fanuc that engraves sequential numbers or a fixed number and the size is scalable. Also a peck drilling macro that feeds down inside a pre-drilled hole prior to pecking and you can specify the first drill depth prior to pecking because many times you don't need to peck until you're 8-10xD deep or so. Also you can specify a pull-out point other than the initial R plane so not to pull all the way out of the hole with really long drills that will snap off when you come out of the hole with the spindle on. I have other ones similar to this that only have the spindle on while the drill is piloted inside the hole. Cheers! Len Dye Fixture Tracking Macro.pdf Fanuc Macros.zip

High Pressure coolant changes the way the material shears so yes it helps break a chip. Stainless steel is still hard to break chips on finish cuts and sometimes a little bigger finish cut helps no make string. Take a look at Chip Blaster website they have some good technical information about HP coolant http://www.chipblaster.com/ Cheers! Len Dye

I agree many think they need to do 5-axis tool paths when many times conventional methods are more efficient, In addition to that, many programmers still use kellering techniques with ball end mill and aren't utilizing the tilt angle formula to allow a flat cutter to cover larger areas on concaved/convex surfaces. +1000 Forum Bonus Points to the first person that can give me the formula for calculating the tilt angle of a given cutter to produce a convex radius that is larger than the cutter?? Cheers! Len Dye

Karl Isn't CP owned by Pankl. Pankl owns part of KTM or did at some time.

that's good to hear that you have it going! Sometimes learning the hard way is the best way in the long run.. This way you'll learn what doesn't work which can be just as important as the way its' suppose to work. Cheers! Len Dye

Ron you wouldn't happen to have any Mori machines would you? I enquired about some machine models and they sell them for a couple of grand now smh

my pleasure Rookie, I enjoy sharing things that work best especially if I inherited it, otherwise I'd patent it first haha I became a "fixture tracking macro" expert by mistake. Many years ago I was sent out to a customer on a new Okuma 5-axis horizontal (5th axis rotary on top of the B-axis) and the customer bought 'fixture tracking software". When it came time to train on it there was no documentation or anything so I called the Applications Manager in Charlotte thinking the software was part of the machine from Japan. NOPE, it was a G-code macro he sent me that someone wrote and no documentation. We loaded the macro up and it didn't quite calculate everything correct and I spent the next half of day figuring it out. Who ever wrote it must of had some experience with it but had never tested it out apparently. After that experience, a 4-axis fixture tracking macro was a piece of cake for me. I've even written one for a 5X tilting rotary on a Vertical as well but on the newer controls you have TCP and TWP now but this fixture tracking macro still works best for me in a production environment. Cheers! Len Dye

I use to train operators/programmers on new horizontal installs for a machine tool distributor and this is what I used to train them on. I exclusively use the WCS Top Front Front tool plane method with just 1 common X, Y & Z origin in MC (i.e., no origin shifts in tool planes for the various B-axis positions) At the machine there is only 1 work offset to establish and the remaining work offsets are calculated from this primary offset using a center of rotation "fixture tracking macro". The beauty of this, the operator only has 1 offset to establish and most of the time its' the same coordinates as the last time the part was ran. This eliminates the confusion on establishing multiple offsets and where they come from. Also it works great with forgings or castings that are going to be a slightly different position each time or where probing for exact position is needed. Here's a document attached I wrote that try's to explain it. Hope it doesn't confuse you its' just something for you to consider starting out in horizontal machining. HTH Cheers! Len Dye Fixture Tracking Macro.pdf

also take note of the diameter symbol on the .2 position requirement. This means that your tolerance zone is a .2 diameter, not a .2 linear distance in either direction. For better clarification get yourself a copy of ASME Y14.5 Dimensioning and Tolerancing standard. The book has examples for just about everything

I would have to agree about a side lock Weldon holder being better for roughing. IMHO, the primary reason is the gage length on a Weldon holder is typically shorter which is vital on a #40 taper machine, particularly on a Haas with relatively small spindle bearing diameter and low draw bar force. Hydraulic, shrink fit holders and power chucks have an excessive amount of overhang with 3/4" and up and retention is put to the test with the cantilevered effect of the load being so far from the gage-line. Higher retention will result in higher tool life as well. Although you must consider a few things when using Weldon holders like make sure you use Weldon spec set screws and flats which have like .004 tolerance across the flats. Also over tightening the set screw stretches the holder body and pushes the tool off center as well. Although you may have some radial run-out, its' less of an issue during roughing because the feed per tooth is high. When your roughing chip load is high like .003, .005 or .008 even .010 per tooth, .001 or so radial run-out isn't kill the tool as much as excessive overhang is. Granted the radial run-out also changes clearance and relief angles that will have an effect on tool life as well. It's all a trade off.. my 2¢ worth... Cheers! Len Dye

IMHO you'd be best to program everything in TCP & TWP but your post would have to support it. Also verify the pivot points on the machine and get them down to .0001-.0002 in order for everything to come out less than .001 true position. If you need to hold tighter tolerances than that then you can always use additional work offsets to fudge those features in. Personally I would stay away from dynamic work offsets and multiple offsets, fixture tracking etc. with TCP there's just one work offset and it makes it so much easier to setup now & months down the road. It's kinda like 2D circle interpolation, it's better to let the control calculate the circle than program point to point, just like it's better to let the control calculate it using TCP or TWP that's my 2¢ cheers! Len Dye

I used to train lathe operators to program home positions using G30 instead of G28 at the beginning & end of each tool. The G30 home position can be set at the machine so that the turret doesn't have to travel all the way home in order to index. On short parts the G30 Z-axis setting may have a value of -250mm. Typically we would have no shift from home position in the X-axis however if you're chasing cycle time you always have that option to reduce the time to index. Also be sure to home U & V first and then W on the next line to prevent collisions with the tailstock or sub-spindle. Furthermore using G30 in your programs allow a more portable program, taking a program from a short bed length machine to a long bed machine, the cycle time is essentially the same. good luck! Len Dye