not sure why it posted multiple times, oops.

Hmmm, sounds like an Okuma MB-5000H would fit the bill. I recall you might know a thing or two about that machine? lol

Hmmm, sounds like an Okuma MB-5000H would fit the bill. I recall you might know a thing or two about that machine? lol

Hmmm, sounds like an Okuma MB-5000H would fit the bill. I recall you might know a thing or two about that machine? lol

Sorry for the long hiatus and the late reply. As YoDoug and Mr. M summed it up, it sounds like for what you are trying to do a schedule program would suit your needs the best. Unlike your Haas, Okuma was smart enough to not make you turn main programs into sub programs just to run multiple files/parts. You can change the display to show the program running fairly easily, I'm sure your frustration is simply due to the lack of training, I assure you the control is far superior and capable than a Haas or even a Fanuc for that matter. What control do you have and we might be able to help a little further.

I highly recommend using the Renishaw macros, however if you don't have the Renishaw macros/software installed here is the Okuma macros for tool setting/breakage. You can change the O# to what ever you like and assign it to whatever library M-code you like, I however typically set them to M201 for tool setting and M202 for tool breakage. Be sure to read the comments as there are a couple of parameters I recommend setting. You will also need to make sure you calibrate the tool setter using the Okuma macros, see the attached sheet for procedure. Let me know if you need help assigning and registering the library files. Save the following into a .LIB file: (************************************) (*****MDI/MANUAL SET TOOL LENGTH*****) (************************************) OM201 (THIS CYCLE IS FOR CYCLE TIME REDUCTION TOOL SETS) (MUST SET PAR NO 36 BIT 3 TO CHECKED MODE) (MUST SET OPT PAR LONG WORD NO 44 TO LONGEST TOOL IN METRIC VALUE=310) (TOOL SETTING) IF [VINCH EQ 2] NMET1 (METRIC) IF [VINCH EQ 3] NIN1 (INCH) GOTO NALM2 NIN1 CALL OO30 VFST=#81H PZRC=0 PFST=1 PUDT=1.0 POVT=.8 PF1=40 PF2=60 PX=VC30 PY=VC31 PRS=VC32 GOTO NEXT1 NMET1 CALL OO30 VFST=#81H PZRC=0 PFST=1 PUDT=1.0*25.4 POVT=.8*25.4 PF1=40*25.4 PF2=60*25.4 PX=VC30 PY=VC31 PRS=VC32 NEXT1 VC30=0 VC31=0 VC32=0 G30 P1 GOTO NEND NALM2 VUACM[1]='CHECK UNIT MODE' VDOUT[992]=2 NEND RTS (*********************************) (*****TOOL BREAKAGE DETECTION*****) (*********************************) OM202 (THIS CYCLE IS FOR CYCLE TIME REDUCTION TOOL SETS) (MUST SET PAR NO 74 BIT 4 TO CHECKED MODE) (TOOL BREAK CHECK) IF [VINCH EQ 2] NMET2 (METRIC) IF [VINCH EQ 3] NIN2 (INCH) GOTO NALM3 NIN2 CALL OO30 VFST=#80H PZRC=0 PFST=1 PUDT=1.0 POVT=.8 PF1=40 PF2=60 PLEI=.01 PX=VC30 PY=VC31 PRS=VC32 GOTO NEXT2 NMET2 CALL OO30 VFST=#80H PZRC=0 PFST=1 PUDT=1.0*25.4 POVT=.8*25.4 PF1=40*25.4 PF2=60*25.4 PLEI=.01*25.4 PX=VC30 PY=VC31 PRS=VC32 NEXT2 VC30=0 VC31=0 VC32=0 G30 P1 GOTO NEND NALM3 VUACM[1]='CHECK UNIT MODE' VDOUT[992]=2 NEND RTS These macros use common variables, VC30=X-axis shift, VC31=Y-axis shift and VC32=spindle orientation. Note that when the cycle is complete the macro will reset the common variables back to zero. With the variables at zero it will act as if tool is on center. In program tool breakage would look something like this: VC30=.25 (X-AXIS SHIFT, THIS EXAMPLE IS FOR 1/2" ENDMILL) VC31=0 (Y-AXIS SHIFT, THIS EXAMPLE WE ARE SHIFTING X-AXIS NOT Y-AXIS) VC32=0 (SPINDLE ORIENTATION, IF YOU TAKE CARE WHEN LOADING TOOLS TO) $ (ALIGN A FLUTE IN LINE WITH SPINDLE ORIENTATION YOU SHOULD NOT NEED) $ (TO USE THIS OFTEN. TYPICALLY ONLY NEEDED FOR ARBOR HOLDERS WHEN) $ (YOU CAN'T CONTROL THE TOOL ORIENTATION) M202 (TOOL BREAKAGE CHECK) Mill_Tool Setter Calibrate.pdf

Here is the STL Check-e incase anyone is looking for it. You need to output in metric (mm) and you need to have the model orientated as you want it to appear. Mastercam will typically do just fine, but you will need to adjust the output tolerance. You want as minimal triangulations as possible. As Colin stated try to dummy the model down as much as possible. Remember this is a primitive tool for simple verification only. If your model has a bunch of holes, threads, grooves, etc. that are irrelevant to the verification get rid of them. I typically try to keep them under 2000 triangles. Another issue people run into is trying to export an assembly. You can only have one model per import. The STL Check-e will verify the surfaces (triangles) and shells (models). There should be less than 3000 surfaces and only 1 shell with zero errors. Play with your export settings until you find one that works for your part. If all that fails, Space Claim works great at healing and reducing the surface count. STLCheck-e.zip

No problem, hope it helps

OK, Super-NURBS & Hi-Cut Pro in a nutshell... First off, please note that Super-NURBS and Hi-Cut Pro will not speed up your program! In fact it will do quite the opposite and slow it down. Here is the best way that I can describe Super-NURBS and Hi-CUT Pro: With either function turned OFF the machine will try to maintain programmed feed as much as possible. With either function turned ON the control will override the feed (acc/dec values) to maintain machine accuracies. Imagine trying to drive you car at 100mph and a sharp 90 degree corner is ahead. Do you smash the breaks just before the corner to navigate in you lane then throttle on as you come out of the corner, if so then Super-Nurbs or Hi-Cut Pro is engaged. Or do you stay on the throttle the entire time and keep the speed at 100mph, cutting the corner then swinging wide taking up the entire road and then some? This would be the results of Super-Nurbs or Hi-Cut Pro being turned off. With that said lets look at some settings; First your toolpath must be CLEAN! I cannot stress this enough. Just because you generated a toolpath DO NOT assume it is good. Actually look at it with a fine tooth comb. Typically when you get jerking the toolpath is to blame. If you zoom in on it and when you think you zoomed in enough keep zooming in, you will see the toolpath jumping around in crazy directions. To help eliminate this I recommend running the filter as tight as possible (I typically run at .0002" or less) and linearize everything. This will cause long regen times and crazy long programs, but who cares the Okuma OSP loves it! For the Super-Nurbs settings (G131 D_ J_ E_ F_ I_ L_ R_ K_ P_ Q_) or For the Hi-Cut Pro settings (G131 J_ E_ F_): G131=ON G130=OFF D= Program tolerance; have this match the filter tolerance in MCAM J= Machining mode; 0=High quality (Super-Nurbs only), 1=Standard, 2=High speed; 0 for fine finishing, 1 for finishing and general roughing, 2 for 3D surface toolpath roughing E= Machining tolerance; this is the allowable error from point-to-point that you can cut the corner (drive across the grass in the example above). Typically I run .002"-.004" when roughing / Semi-Finishing and .0002"-.0004" when finishing F= Feedrate upper limit; This will not increase the programmed federate! it will only limit the max, similar to a G50 S___ on a lathe. If the operator turns the federate override to 200% that could cause damage to tool/part/machine. By setting this value you can limit the allowable override. I typically always set this at 1240. since that is the fastest I have ran a tool in material to date. I= Utilize Reconstruct Shape; 0=Low, 1= Medium, 2= High, 3= Full; Since I typically set my program filter tolerance very low (0.0002") and linearize everything I do not need the OSP control to reconstruct the point as much as I would need if there were spline segments. So I typically have this set to 0 (Low), if there are any splines I would either re-create geometry to select from or set this to 2 (High) or 3 (Full). L= Max block length; Default (20.0mm or 0.7874") R= Min. block length; Default (0.3mm or 0.0118") K= Program filter mode; Default (Off); 0= Off, 1= Mode 1 on, 2= Mode 2 on, 3= Mode 1 & 2 on; If you toolpath is clean, you should not need this enabled. However, if you still have toolpath that jumps around you may need to enable this function. P= Filter value length; Default (0.01mm or 0.0004) Q= Filter value angle; Default (5°) I hope this helps, also please refer to the manual for additional information. Super Nurbs.doc

TurnCut is an awesome feature and works great for the mostly mill part that needs a turned feature. I do not believe mcam has a cycle dedicated to this, but you could create a custom drill cycle to output the code needed.

No problem. Let me know if you need any other help

Do you have the Renishaw probing macros installed? If you do here is the Renishaw Inspection Plus manual that has all of the cycles. It is pretty well documented. Inspection Plus_H-2000-6550-0C-A.pdf

If you do a lot of ballmill/spline surfacing I highly recommend Super-NURBS. I would also recommend Fixture Tracking (CALL OO88) if you are planning on running 3+1. If you plan on running small tools at high RPM (12k) for long durations I would also look into a coolant chiller to keep the temp stable. You will get better finishes and hold tolerances tighter. The machine can only control and compensate for the machine growth/shrinkage itself, keeping the work material and workholding from thermal growth/shrinkage is just as important for some.

Make sure you get the Renishaw Set and Inspect app installed, it is very user friendly and helps shorten setups.

Here is a brief rundown of OSP vs FANUC The G116 tool change call is a custom macro in a .LIB file format that is assigned to a macro G-code. If you do not have this you can use T# M6 (Traditional Oxxxx program number not necessary) (The CNC machine will recognize the Windows file name as the program name) (the file extension MUST be .MIN for a main program and .SUB or .SSB for a sub program) N2 G116 T2 (Tool call. T# M6 is also valid for calling tools) G15 H01 (this indicates work offset #1, or G54 in Fanuc) G0 G90 X-13.535 Y8.0 S8000 M3 T9 G56 H2 Z.25 M8 (G56 is command to read tool length offset. Fanuc G43) Z0.02 G1 Z0 F100. X-11.135 F90. Y0 X11.8 G1 Y8.0 G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0) M1 N66 G116 T9 (Drill) G15 H01 (Work offset) G0 G90 X10.593 Y33.7878 S7000 M3 T1 G56 H9 Z15. M8 (TLO read) Z.25 G71 Z2.5 (optional- set a clamp clearance point) G83 M53(special retract- Fanuc G98) X0 Y0 Z-.5 R.1 F38. (all codes same as Fanuc) CALL O1234 (Cal sub for modal hole drilling- Fanuc M98) G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0) M1 N66 G116 T1 (spot Drill) G15 H01 (Work offset) G0 G90 X10.593 Y33.7878 S7000 M3 T10 G56 H1 Z15. M8 (TLO read) Z.25 G71 Z2.5 (optional- set a clamp clearance point) G81 M53(special retract- Fanuc G98) X0 Y0 Z-.15 R.1 P1. F38. (all codes same as Fanuc- P=Dwell) CALL O1234 (Cal sub for modal hole drilling) G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0) M1 N66 G116 T10 (bore) G15 H01 (Work offset) G0 G90 X10.593 Y33.7878 S7000 M3 T15 G56 H10 Z15. M8 (TLO read) Z.25 G71 Z2.5 (optional- set a clamp clearance point) G85 X10.322 Y31.8297 Z-1. R.1 F20. M53 (Same as Fanuc) CALL O1234 (Cal sub for modal hole drilling) G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0) M1 N66 G116 T15 (rigid tap) G15 H01 (Work offset) G0 G90 X10.593 Y33.7878 S3000 M3 T16 G56 H15 Z15. M8 (TLO read) Z.25 G84 X10.322 Y31.8297 Z-1. R.1 F166.66 M54 (Same as Fanuc-M54 means return to R plane. Fanuc G99) CALL O1234 (Cal sub for modal hole drilling) G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0) M1 N66 G116 T16 (rigid peck tap) G15 H01 (Work offset) G0 G90 X10.593 Y33.7878 S3000 M3 T2 G56 H15 Z15. M8 (TLO read) Z.25 G283 X0 Y0 Z-.5 I.075 R.1 Q.1 F166.66(G283 is a peck tap. I=retract amount, Q=depth of peck) CALL O1234 (Cal sub for modal hole drilling) G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0) M1 M2 (Or M30) O1234(Sub) (Subs can be either in a separate file or attached to the main program) X1. X2. X3. X4. RTS(Return to system. Fanuc M99)

if you enable shortest direction and force to output every quadrant that solves the 0-180 direction issue. It would go 0-90-180 or 0-270-180.

Sorry for the delay in response, I have not been on here for quite a while. I believe Okuma does offer a gantry loaded for the Multus, but it may have the same downfalls as some of the others with limited gripping force to handle the size/weight. You said it is Ø5.5" bar, but what would the slug length be? and the weight? We also have a full automation team that can integrate Fanuc or other brand robot loaders. Another popular option is a robot with a drawer system. It creates a very compact and efficient setup. We have an Okuma Multus U3000 located near you, in Tualatin, if you would like to view. BTW... is this Eric, previously at Turk?

Renishaw Axis-Set IS available for Okuma lathe controls, but I'm not sure if it is compatible with the older OSP-7000L control. There are a lot of new system variables that the macros read from and write to. I'm sure with some tweaking we could get a version suitable for your machine. Have you tried contacting our local office? 714-446-7770 for our SoCal office.

Have you looked into the Okuma Multus U3000? CNC Software has a M/T Okuma certified post available. We have one that we can show local to the Portland area.

The Multus B300 is a great machine but as mentioned earlier it is not a true Y-axis, it does have a compound slide. The Multus U3000 has the a true Y-axis and in my opinion a lot more robust configuration, although both machines are great. My only real suggestion whether you go with an Okuma or not, BE VERY CAREFULL IF BUYING A USED MACHINE!!!! I cannot stress this enough. There are a lot of good deals to be had in the used market for most machines. These types of machines however are a different story. I strongly recommend and urge you to look only at new machines. There are too many components and variables in this class of machinery. I personally have seen a shop buy a used machine to turn around an invest more than the cost of a new machine trying to restore it to factory specs and still has issues. If the machine has been crashed there can be a lot more damage and alignment issues than what can be seen from a basic inspection. My 2 cents for what its worth.

Chris Kozell at CNC Software has a solid MT post as well for the Multus line.

SAH-WEET! That is exactly it. Never noticed that until the PB must have installed without it enabled.

I know, I'm not blaming Mastercam for this one, although if I could select the level that the solid is in it would eliminate a couple of steps.

Did anyone else notice in 2018 PB and PC1 you could toggle the visibility of the active level, but in the final release they took it away. I actually liked that feature, it came in handy to not have to change my active level just to hide it for a short bit.

Ahhh, in the Tool Manager you can only import a DXF, but in a operation you can import the solid model. Now, only if all the STEP files were orientated correctly. You still can not select a level that has the solid model. So now I need to open each STEP file, reorient and export just to import again. Grrrr this is a little frustrating.