Threadmilling can be done quickly with the threadform form ground into the OD of a typical endmill or for just to get it done ( like now ) Use an internal threading bar from a lathe with the correct threadform tip installed -use 2D contour-ramp ( ramp = thread pitch ) ( perpendicular lead in / out ) ( caution if using arcs ) ( RH thread starts from bottom moving CCW, feeding out ) ( rotate the bar at the correct cutting speed ) ( feedrate controls finish not the pitch and can and will be quite slow ) This method can be used on internal and external threads with the same tooling but it will be a lot slower than turning. unless your machine supports turncut function Turncut example

"You may also need to remove the "G95" call as well. Like I said, make a back up and be careful. " Adding to previous post If changing your machine to feed per rev ( G94 ), I suggest you turn it back to feed per minute ( G95 ) at the end of the cycle, usually after the G80 or G00 line (for safety). Facing or contouring at 3" per rev may be a bit fast for any machine

Try setting all WCS and planes to TOP when running Verify and then save the STL file Even when your "compsre to STL" is used, check the position of your checking file before comparing Your WCS is the real killer

When setting your views and origins in "view manager"- goto Work Offset and place the number you require in this field This number will be recalled when this view is used - you will also find this number will be shown at the end of the parameter line in each operation if greater than ( -1 ) If using different work numbers for the same set-up i.e. set w/off# in view manager to TOP=1, FRONT=2, BACK=-1 WCS=TOP Tplane=TOP w/off #1 - outputs #1 WCS=TOP Tplane=FRONT w/off #2 - outputs #2 WCS=TOP Tplane=BACK w/off #-1 - outputs #1(by default) This is not a permanent setting for Mastercam only for this file If it is required as a permanent setting, your post will require adjusting, quite often "Misc Intergers #1" is used forthis feature mod.

Have you rechecked your WCS & planes ? Have you programmed in TOP for a horzontal and then trying to machine at other planes thet may not be quite correct ? I've had a similar problem where tool retacts after each op. on an incorrect set-up (plane) Verticals -WCS=TOP T/plane=TOP, FRONT, BACK etc Horizontals-WCS=TOP T/plane=FRONT, LEFT, RIGHT etc

You could create a directory as your save version to place the files without having to alter the filename, this structure will show up in your filepaths ie. ..MC9, ..MCX, ..MCX2, ..MCX3, etc. It will indicate minimum version required to open the file

Try using 'Contour (ramp)' plunge - depths controlled by ramp depths - you also get cutter comp control G41 and G42 outputs - you can also use multipasses your contour is centre line of tool with comps 'OFF' your contour is your profile if comps required Just make sure start and end points do not descend onto material Steve

Is it a thru or blind hole ? Interpolate start of hole (.001" under reamer size )to true hole positions Use reamers that push swarf into thru hole into uncut area ( suggest using cutting oil not coolant ) DO NOT rapid retract -( 4X feed )

We have Okuma MX55 with A-axis Our MC will not go past 27 rotations as well this is a machine software limit I suggest checking with Okuma to change MC settings so that the control will reset 360 deg. back to zero on each rotation also change A-axis parameter to travel shortest distance Your post will need a small modification to output correct code **I mean only small**

Cutter comp is a real bitch at the best of times, but if you were to leave it on between operations then the rapid to points would not be correct You would have gouges and comp. errors at every operation ( even more if using multi-passing and/or depths ), a big problem in tight spaces As the others have said, - rapid to point ( this point would alter if comp is on ) - descend - comp on ( usually using lead-in line ) - contour - comp off ( usually end of lead-out line) - retract using 'conrol' ( comp = tool radius) or 'wear' ( comp = zero ) method - what you get on screen is close to reality ( uses G40/G41/G42 ) using computer method - is real ( t/path is not adjustable in machine ) ( no Gcode comps output ) Yes, hold your position let Mastercam output safe code If they want it their way ( manually edit and physically prove out the program ) Just a note, if you let mastercam run their way, who would get the blame for the gouges ( Mastercam? ) To run their way, use 'computer' and let them add the codes

Michael, Hi Thanks for your comfirmation that the standard way won't work. The newer "ISCAR" feedmills, I have changed my attack to having them as facemills, as for the older ones, they will have to go as bullmills ie, standard feedmill OD 20mm with base dia. of 6mm and main radius of 11mm is defined as 'bullmill' OD = 28mm, corner rad =11mm ( custom shape, I agree, will have to be played with, and **note** it is only a representation not the actual cutting shape) ** As to verifying your tool and path - check against a STL model in verify ** The special finishing tool I'm using ( 12mm OD with R12 nose ) is now done with 24mm ballnose, just have to modify my boundries. This is one that will have to go thru "VERICUT" Thank You Michael and All Steve

gcode- the tool profiles all start at X0 Y0 and chain to finish at the X0 line Problem is that the form of the tool when stock allowance on drive and check surfaces are set to zero, the tool is stil a loong way off the part ( even more if I have allowances ) It appears as if a bullnose cutter is being used when a ballnose is the tool Picture a cylinder ( side view ), the tool would touch only at the quadrant points ( top and sides )

A suggestion for any tapping is to set feed per rev before tapping cycle so that your feedrate = programmed pitch , then the operators can adjust RPM in the program without affecting the pitch ***DON'T FORGET G94*** turn feed per minute ON as most millers like feed per minute or your next feed move on the part wil be v________e________r________y quick Core drilling sizes for spiral taps are very different to roll taps ( roll tap core sizes must also be tightly controlled ) When tapping into SS-304 , take the core sizes to just under the highest size permitted. Cutting speed for tapping 1020 @ 7-10 m/min for M6 * 1.0p = S300 > S600 ( can go higher ) can use coolant or compound Cutting speed for tapping SS-304 @ 4-7 m/min for M6 * 1.0p = S200 > S400 ( can go higher ) use compound Spindle is NOT started at RPM line as to keep tool in sync, even if it is toolchanged example code for OKUMA G15 H1 G0 X0. Y0. S300 G71 Z2. G95 M00 ( BLOWN DOWN and APPLY CUTTING FLUID ) G284 Z-.5 R.3 F.04 M53 ( g-code starts RH rigid tap cycle ) X1. Y0. X1. Y1. X0. Y1. G00 ( or G80 = cancel cycle ) G94 (**** note ****) M9 M5 G30 P1 M01

Tool is showing itself correctly in backplot and verify and our systems are set to show tools "as defined" this toolpath is set for cutting in a 3-axis machine setup before passing onto a 5-axis machine for swarfing and holes PX this is an "aero" part so I can't play with it at all.

Thanks for the quick repy Tool profiles are only lines and arcs ( splines not used in any profile to eliminate problems.) I had a quick attempt in V9 again, I am getting same result now as in X2 ( not good ) Last resort will be doing the t/paths with standard profile tooling ( facemills, ball bullnose - all on steroids ) Tools I want to use are "ISCAR FEEDMILLS" and special finishing tools to increase stepovers ie. 12mm endmill with R12.0 ground on the face with R1.0 corner fillet ( sorry guys - we're metric down-under ) Picture a 24mm ballnose, now grind the flute OD to 12mm diameter and break the corner with R1.0 ( this is my finish tool )

G'day all, Help required on custom tools in X2. they are not working out the same as in V9.1 In V9 I had success with custom tools (on or near to) touching curving surfaces But for the life of me I can't get any tools to do what I tell them to in X2 ( not so strange an event). I'm using same comps and tool settings used in V9 and have tried:- - undefined tool with custom profile ( drawn full size ) - endmill / ballnose / bullnose with custom profile ( drawn at scale that Toolrad = 1.0 ) I have drawn tools correctly ( frmm 0,0,0 in X+Y+ quadrant, no c'line, chains OK, no duplicates, on it's own level, and so on..) also tried having tools embedded in the current MCAM file, and as they all display OK in backplot and verify. So this is not the problem area ------ but bugger me ---- it still won't *@!#% work I am having problems loading my package to the FTP site ( under construction ) as usual it's a job required Yesterday ( 1 week ago ) Any input is welcome Thanks all in anticipation