Software policies with nearly all software companies change as do partnership agreements from time to time. I merely wanted to correct you in case someone took what you stated as policy and were prepared to make a decision based on that statement. As always, it is best to contact YOUR software provider regarding policies and pricing rather than rely on Reddit, eMastercam, Practical Machinist, CNC Zone, etc... for accurate up to date information. Many unlisted factors go into pricing and policies.

I think you may have been misinformed on the pricing. Yes there is a per-user license, there is no "per-machine" cost to the best of my knowledge. We have a number of customers with 5+ machine tool builder variety with multiple machines from each builder and they only pay the per user cost. While true there is no actual "floating" license, I personally manage 12 (IIRC) licenses between 15 to 20 users. I have no trouble or issues doing it. I assign and revoke as needed. It takes maybe 30 seconds.

So far the Autodesk acquisition of CAMplete has been no factor. The only kind of negative so far is bug fixes and feature enhancements are mostly on a schedule now. That said, the subscription only model isn't great. I like to own stuff, not lease it. However the product is phenomenal and is a way better posting solution than anything else out there. Several updates per year now is how it is as opposed to how it used to be, but, I haven't run into any show stoppers so it's fine. There's always a work around... just like Mastercam. The AD haters were predicting doom and gloom for the product. They pretty much look like we all did when we predicted SolidWorks' demise... WRONG!

Actually yes it can. And it's been able to do so far years.

It just won't simulate. When I have proven probing cycles that's what I do... Manual Entries.

Yeah. The only way to get probing into CAMplete and have it simulate is to program it with Fusion360 or CAMplete's clunky probing stuff (which I never use). Double check with your PQI guy that they set up the (REN*FCS*TO*WCS) (usually in O9744 but PQI does some funky stuff where they deviate from the Renishaw standard with their Renishaw InspectionPlus installs). (************************) N30 (FCS*TO*WCS*CALC) (ONLY SET WCS FOR TABLE TYPE ROTARY AXIS) (ALL TOOL TYPE ROTARY AXIS = 0) #1=0 #2=#5024 #3=#5025 Set your tilt and rotary variables based on A/B, A/C, or B/C configuration. The above example is for a B/C kinematic machine. #5024 = Machine Coordinate for 4th Axis #5025 = Machine Coordinate for 5th Axis If your Yamazen AE can't answer your questions, hit me up.

If you're using CAMPlete for post processing, the CIMCO Probing package add-on is not compatible with CAMplete. Send me your PQI InspectionPlus manual and I can modify the Fixed Sentence file and you can read it in. It's got some extra goodies in it as well.

@Kyle F Have PQI modiy this to suit your machine then upload this Fixed Form Data to your machine. This is an easy way to create In-Process measurement cycles into an existing part program. FIXFRM_MX-iHMI.DAT

If you go the the maintenance tab on the Matsuura overlay, go to the.... maybe WEEKLY button... then right arrow soft-key to IPC PARAM soft-key. A table shoud show. In the upper right corner of the FANUC section of the screen you'll see PAGE x/x. It's either be x/5 or x/4 or x/3 (unlikely) the "x" being 1, 2, 3, etc...

The Series and Edition are up to spec to support the Matsuura software update... G423 and 49.0 are the minimum. You're at G423 and 69.0

Page up from there... we need to see the CNC System Series and Edition.

That's not the "software" series and edition, that's the "control" series. Go to the parameter screens, right arrow soft-key over to the "SYSTEM" soft-key. You should see something like this; CEXEAPL FR32 0009 CEXEDATA0 FM51 03.0 CEXEDATA1 FM10 17.0 CEXEDATA4 FM09 38.0 EMBED ETHER 658M 23.0 USB SOFT 659A 05.0 ETHERNET 658K 25.0 IHMI(SYSTEM) BX72 0019 IHMI(MACROM) BX72 0019 ETHER/DTSVR 6569 32.0 Page up maybe 1 or 2 screens 2.SOFTWARE CONFIGURATION SYSTEM SERIES EDITION +------------+--------+--------+ CNC(SYSTEM1) G423 35.0 CNC(SYSTEM2) G423 35.0 CNC(SYSTEM3) G423 35.0 CNC(SYSTEM4) G423 35.0 CNC(MSG1) G423 35.0 CNC(MSG2) G423 35.0 CNC(MSG3) G423 35.0 CNC(MSG4) G423 35.0 CNC(MSG5) G423 35.0 BOOT 60WH 0001 This is what I need.

High Speed modes should NEVER be active during probing. EVER!

FANUC doesn't install the Matsuura software ever. What Series and Edition was installed? It should be on the FANUC service report. PQI does not update Matsuura software. They may install Renishaw iHMI. Productivity "might" be able to. If anyone else besides Matsuura or I can do the Matsuura software it would be Productivity.

Between the MTB stuff in the \\CNC_MEM\SYSTEM\ , \\CNC_MEM\USER\, and the \\CNC_MEM\USER\LIBRARY folders.... MTB stuff, tool measurement, spindle probing, user MACRO programs, etc... should take up less than 500kb, leaving at least 7,500kb free space. My personal opinion is ALL part programs should reside and run from the DATA_SV. This provides one with the possibility of network backups which on CNC_MEM isn't possible... at least not the same way. HTH

G05.1 is VERY picky about what is modal in activation/deactivation. If I were a betting man, something is activated in your G510 MACRO that needs to be canceled. If you don't have access to the MACRO, cancel EVERYTHING between operations. G00G17G40G80G90G94G98 G49G53P1Z0.0S11460M03 N30001(Contour Back Edge for Inspection Surface - 3:00 Face) G05.1Q1 G00G90G54... G43Z4.0H#517 ... G40Y2.5625 G00Z4.0 G05.1Q0 G00G49G90G53P1Z0.0 I would try activating the G510 after the G54 or after the G43, the deactivating either before/after the G05.1Q0 or after the G49. That's where I'd start. Be careful with G49. If parameters are not set correctly, you will get a Z- move the equivalent to the length of your positive tool length offset. HTH

You've run the same program, the same way on both CNC_MEM and DATA_SV? 300kb is nothing. I routinely run programs 3-4x that without the stuttering you are describing. A note on DATA_SV management, I have seen a performance degradation when there are "a lot" of programs in the root DATA_SV. I always recommend customers to use folders and sub-folders. I don't have a definitive number of programs when the performance degredation starts unfortunately. It was just something I noticed accidentally. So I typically reccommend \\DATA_SV\CUSTOMER_NAME\PART_NUMBER\REV\ for a structure. This keeps things clean. organized and running smoothly... in my experience anyway.

M203 M08 M132 can all be in the same line. This would ONLY apply to 5-Axis Matsuura machines WITH touch panels AND built after 12/2021.

Ok, you're probably up to date on code formatting. Touch panel machines built after 12/21 can do multiple non overlapping m-codes on the same line, and have a few other pretty awesome functions. Depending on a number of programming paths, plane changes and canned cycles, I've seen 20% reduction in cycle time old vs. new. Sometimes more. Matsuura does have a software update available for the 5-Axis machines built prior to that date. It's not free - I have absolutely no idea of the cost so don;t ask. I don;t even know the ballpark number unfortunately. I do know FANUC and the Matsuura factory needs to get involved which is why it costs. Me, I'm trained to do the Matsuura side software update (I believe I'm the only non-factory guy in the US that can do it) but FANUC needs to come out and update the CNC System Series and Edition software. See below for the machine's requirements top be eligible for an update. In order for any 5-Axis Matsuura to receive this update it must have the following; FANUC-31i-B5 Control Panel-i or iHMI interface FANUC System Software Series G423 or greater FANUC System Software Edition 49.0 or greater Software from Matsuura Software installation from Matsuura (or a factory trained engineer). If items 1 or 2 are not true, then the machine cannot get the update period. If items 3 and 4 are not true, the machine dealer must issue a request to Matsuura USA, Matsuura USA must issue the request to FANUC to update the System Software to the minimum required for the update and Matsuura USA must issue the software request to Matsuura Japan. There would be a charge for the FANUC trip, how much depends on location; the 3 tiers for travel are less Than 4 hours, 4-8 hours, and 8-12 hours. Not sure what Matsuura is charging for the updates. Probably depends on proximity to Minneapolis, Minnesota.

Probably not too far off. This is my latest 3+2 format (for 5-AXis machines built after 12/2021 or machines with the Cycle Time Reduction spec software upgrade); #996=0.75(CAM TOOL DIA.) N2T2M06(0.75 in squareend assembly) G00G17G40G80G90G94G98M132 G49G53P1Z0.0T1M08 N30001S11460M203(OPERATION COMMENT HERE) G05.1Q1 G00G90G54B-90.0C-180.0 G54.4 P2 G68.2 X0.0 Y0.0 Z0.0 I-90.0 J-90.0 K-90.0 G53.1 X-0.053Y2.0834 G00G43Z0.702H#517S11460M03 G05.1Q3X0Y0Z0 G00Z-0.2979 G01G41X0.2652Y1.7652D#517F120.0 ... G01G40X0.0601Y2.1824 G00Z0.702 G05.1Q0 G00G49G90G53P1Z0.0M229M205 G69 G54.4 P0 G130 (INSERT TOOL BREAKAGE CYCLE HERE IF DESIRED) M05 M09 G00G17G40G49G80G90G94G98 M01 5-Axis w/3DCC; ( *) #996=0.0313(CAM TOOL DIA.) N5T5M06(Tapered tool assembly) G00G17G40G80G90G94G98 G49G53P1Z0.0T6 N50020S12000M203M132(Flow ISO-TC39SC2-N2185 Feature - Side 1) G05.1Q1 G131F1 G00G90G54B-29.755C122.76 G54.4 P2 G68.2 X0.0 Y0.0 Z0.0 I212.76 J-29.755 K-90.0 G53.1 X-0.4636Y0.5398 G69 G43.8Z1.2495H#517D#517S12000M03 X0.0994Y-1.152Z0.8547,L2I0.5411164J-0.840937K0.004251 X-0.102Y-0.839Z0.2035,L2I0.5411164J-0.840937K0.004251 X-0.1423Y-0.7764Z0.0733,L2I0.5411164J-0.840937K0.004251 G01X-0.1611Y-0.7472Z0.0125F9.0,L2I0.5411164J-0.840937K0.004251 ... X0.1438Y-0.1655B-22.642C-293.154,L2I-0.3899529J-0.9118848K0.1280734 G00X0.1048Y-0.2567Z-0.1284,L2I-0.3899529J-0.9118848K0.1280734 G05.1Q0 G00G90G49 G49G53P1Z0.0 G54.4 P0 G130 M05 G00G17G40G49G80G90G94G98M229 M01 5-Axis w/CC ( *) #996=0.1875(CAM TOOL DIA.) N4T4M06(Tapered tool assembly) G00G17G40G80G90G94G98 G49G53P1Z0.0T5 N50018S12000M203M132(5-Axis Swarf Side Rough +.005 on wall) G05.1Q1 G00G90G54B-1.016C-5.894 G54.4 P2 G68.2 X0.0 Y0.0 Z0.0 I84.106 J-1.016 K-90.0 G53.1 X0.039Y0.1389 G69 G43.4L1P3Z0.8589H#517S12000M03 G131F1 X0.0379Y0.1358Z0.8602 X0.0511Y0.1344Z0.1103 X0.0537Y0.1341Z-0.0396 G01G41.2X0.0549Y0.134Z-0.1076D#517F90.0 ... G40X0.0476Y0.1333Z-0.1088 G00X0.0356Y0.1512Z0.859 G05.1Q0 G00G90G49 G49G53P1Z0.0 G54.4 P0 G130 M05 G00G17G40G49G80G90G94G98M229 M01

Could be worse... could have had to identify as a Gender Changer.

What's the manufacture date of your machine @SuperHoneyBadger?

We have a lot of customers that do very well with their Haas machines. They understand what the machine is and what it isn't and work around it.

You bought a completely different class of machine, it SHOULD have been an amazing difference. Yours is not a typical experience. If you would have bought a Matsuura you would have never even looked at a Mori so there's that.

The opinion probably came from the early days (pre- [b]i[/b] Series Controls) when because the function was called "look ahead" and there were not any levels attached to it. It was either on or off. So, it was thought there was no benefit to a "look ahead" for positioning type tool-paths because it was just going from A to B and it wasn't performing any contouring type motion. But with modes and levels, you gain some functions.