On 4/24/2024 at 4:38 PM, Kyle F said:

I've never had an issue with the mastercam 5 axis link. Generally I'll prove the program out with forced tool changes between each multiaxis path and then once I have them all dialed in I'll go back in and add the multiaxis link. Then go re-prove it out again lol

I typically do not use those 5-Axis linking strategies, or if I do, I use them sparingly. Transition from operation to operation can be tricky. You can get wild unpredictable motion. Much of the motion is dictated by machine parameters (wind/unwind/rotary axis rollover, etc...)

In a multi-pallet production environment where unattended operation is the main goal, safe and predictable is your friend.

The OP @Tommy Thompson last visited this topic on Tuesday...

The only real drawback to utilizing the multi-face approach is that you'll have more tool changes. So 4 tool changes over 4 parts as opposed to amortizing 1 tool change for 4 (or however many) parts. 

My personal primary preference is flexibility. There is more to "cycle time" considerations than from program start to program finish.

Like if the machine is running 24-7, NEVER idle, then yeah, you want that cycle time to be as short as possible. If your fully loaded machine runs for 2 shifts then sits idle for one shift, then really you gain nothing by shaving every millisecond off the cycle time because that time savings was killed by the idle 3rd shift. 

"There's no perfect solutions, only compromises." Thomas Sowell

What the pre-position does for you is create a safe and known transition from path to path. 

If you want sexy, YouTube worthy machine porn, there's a path in Mastercam (5-Axis Linking) or CAMplete's Auto-Link function (it requires an NC Format that supportsthe function. It has to be turned on also... by default it's off.

If you want to know how to turn it on, let me know. 

Even though we use CAMplete, maximizing the use of the available options on the machine took a little work. 

Currently I'm working on utilizing the tolerance control feature (G10.8). That's gonna take a bit.

If there's anything you need for the Matsuura just ask. 

Glad to help wherever I can.

It's a lot to take in, but getting a dialed in post helps. 

I was having a discussion with someone last week and they contended that knowledge of "g-code" isn't useful anymore because of CAD/CAM. 

I only partially agree with that statement. Does someone need to know how to write a program from scratch? Meh... not really. What someone that works with or writes programs MUST know is Program formatting. When to turn things on and when to turn them off. When to use this function, and when to use that function. While a dialed post can solve some of those issues, when a company gets a new machine or the machine has options that are unfamiliar, being able to troubleshoot code formatting is a critical skill. 

At then end of the conversation I thingbwe agreed on most points. 

So on the MX (or any multi-pallet Matsuura) in the pallet manager you can assign up to 4 programs to the pallet. It can be 4 or the same programs or 4 different programs. Doesn't matter. 

When talking pallet manager with customers I always go over a number of scenarios. Aluminum and easy to machine/non tool-eating materials tool path transform with multiple parts in the same program is typically fine. More difficult materials or materials that generally wear tools out or break tools, I reccommend separate programs that way when using tool life management you don't have to kill the whole pallet to flag the tool, you can just flag the face. Then the face is flagged and will continue to the next face and pick up the backup tool. 

G68.2 in a nutshell allows the part's coordinate system to follow the part around regardless of the tilt or rotational axes orientation. So X0, Y0, Z0 is X0, Y0, Z0 always no matter what. 

That's the basic explanation.  There's a little more to it under the hood but that's basically what's going on. There's no need to even consider center of rotation, and it's better if you don't program to it. 

Writing the errors is just a matter of how you want to do it; by G10 or by variable number/variable name. 

By variable Number;

https://www.dropbox.com/s/5f25nw9rg0nfrbu/WSEC Variable Table - FANUC 30i.pdf?dl=0

By G10

G90G10L23P = P1 – 7=P7 (x, y, z, a, b, c, and possibly a Tilt and a Rotary Axis)

On 4/19/2024 at 10:47 PM, Tommy Thompson said:

We have a number of fanuc controlled vmcs from various machine tool mfgers. Most are oi-mf. The machines are generally great and the controls usually perform well but our shop is struggling to load the new high speed machining tool paths or multiple programs for part arrays onto the fanuc machines.

1)Without engineering know how, adding memory or ftping or getting a control to recognize a cf card in an adapter to a pcmia port (must be the last place on earth for such a thing) is all extremely time consuming and frustrating.

2) The tiny memory on the average fanuc control is hard to understand. I’d like to know why they do not just put a tb of memory on these machines

3) or make them connect easily to a computer.

4)It seems like it takes patient dedication or an cs degree to make them work.

5)Endless nuance about partitioning cf cards, etc.,embedding ethernets.

6)It might be fine for a large firm or some of the wizards out there, but for the average job shop, it’s a failure.

7)If you are an engineer who speaks fanuc and wants to earn some money please let me know.

8)If you want to say it’s a piece of cake, save it bro. 

Lots to unpack there so without further adieu...

1) FANUC Program Transfer Tool (available https://www.fanucamerica.com/products/cnc/cnc-software/programming-simulation-software/program-transfer-tool for under $30 USD) . I use it and reccommend it HIGHLY. CF Cards MUST be 1GB or under for 30i/31i/0i-F series controls. I keep a 128MB (yes you read that right) card for older era machines. I get mine from Amazon. I like these for 1GB's https://www.amazon.com/1GB-Compact-Flash-100X-INDUSTRIAL-Pio/dp/B000ZNWOSS/ref=sr_1_2?crid=I99RBMCIPDWH&dib=eyJ2IjoiMSJ9.vy01M8EQ4MyyBDSDjeq_NuppS6M0tWgWrlcoasmKUzHjiYMoBe4U0bq62scns-U3Z0sxEMsM4q6X_kTLHXLVeZIRbO48o0Ipi--Hbq_FKm_aXz3hHfnB-91bIoKmwAUB53WTZHmRWTDJUWArvdnEuFhSkXyZiuemWcvM7BHOfMdrt8mszRDnM4pnfYkaWH1zERpJt7BhJnTVxO8zVuM1eqnIyDCY6XJQqDZxH8O15pWTx-OlI9AUfeXcdAxgw5UvrmuowILrWHeEtGMuZOhPyXp7I7NocgDEelaG2jZaAnk.d2rRem4np6HQzDANiXqa6evpgkauOin78IjLz0UNivw&dib_tag=se&keywords=1GB+CF+Cards&qid=1713845397&refinements=p_n_feature_five_browse-bin%3A673261011&rnid=673240011&s=pc&sprefix=1gb+cf+cards%2Caps%2C126&sr=1-2

It's only frustrating if the company you bought your machine from is not knowledgable. Support matters. Especially today.

2) This is NOT a FANUC issue. This is 100% on the machine tool builder. We spec our machines with 8MB of CNC Memory and 1GB of Data Server Memory. The latest machines have SSD Drives with TB's of storage and they are FANUC so... the problem isn;t with FANUC it's with your builder improperly specing a machine. Assign blame wher it belongs.

3) See #1

4) I barely graduated high school... and by barely, I mean if it weren't for woodshop and PE I woudln;t even have had a 2.0 GPA... and I have no trouble connecting machines to networks if they are equipped with either an Embedded Ethernet port or a Data Server. Been doing it since the 90's. You need better machine tool support.

5)I've not been successful partitioning CF Cards lately. Like for the last 10 years lately. Just get a 1GB CF card or smaller with a PCMCIA adapter and it'll work. Embedded Ethernet is a simple setup. EIther use DHCP or set a static IP address, set the router and DNS IP Addresses, plug it in and it works. Just to prove a point to a customer, I went out to Home Depot, bought a Wireless Extender with an ethernet port, set it up, set the control for DHCP, set the router and DNS, restarted the adapter and I was able to ping the CNC form anywher ein the shop. Once I was connected to their network, I coudl upload and download programs at will.

6) You just need better machine tool support

7) I give away my knowledge for free. It's worth plenty, but so many gave to me freely, I'll give freely until I get burned.

8 ) I will say it's easy, because it is. I'm NOTHING special. Believe me. I'm just an average at best guy. Your machine tool dealer has a high degree of incompetence, or they are withholding support from you. Either way, I'm sorry you are going through this trouble. You should not have to suffer because of your machine tool dealer is incompetent or your machine tool builder didn't adequately option their machine.

I hope this helps.

On 4/20/2024 at 4:06 PM, Kyle F said:

...IIRC our matsuuras have 1gig of internal memory on the data server but I've only loaded a handful of small programs so I haven't even had to go that route yet.

Put ALL your pat programs on the DATA_SV. Just use CNC Memory for custom G/M-Codes, Custom MACROs, etc...

8 hours ago, Kyle F said:

At my shop we recently dove head first into automation, got a mx-330 pc10 and mam72-52v. I've been running the MX for a few weeks now lights out and I have to say it's been a breeze.

.....

it's surprising how little you have to raise your workpiece off of the table for access.

...

This is one of the many areas I believe Matsuura is FAR superior to the toilet bowl lovers in machine design.

Matsuura can get closer to the pallet center with the head/spindle. Doing this allows you to run shorter tool assemblies and it requires shorter work holding to get ot he part. All that to say a more rigid machining setup = the best metal removal scenario possible.

8 hours ago, jas6142 said:

The matsuura dealer will be in here Monday .   I see they now offer the mam in a 45v which is about the ideal size, last i knew they only offered the 35v.  ive always been partial to the mam's for the automation.

In the MAM series they offer the MAM72-35V, MAM72-42V, MAM72-52V, MAM72-70V, and MAM72-100H. Then in the CUBLEX series there is a CUBLEX-35 and a CUBLEX-63. There was a CUBLEX-42 but I believe they discontinued it.

350mm, 420mm, 520mm, 700mm, and 1000mm respectively.

The number after the dash is the CM value of MAX pallet Changing swing diameter essentially.

Also, if you've got the inspection stuff squared away, it's easy peasy to generate reports, csv data, etc...

If you can imagine it, you can format it, and generate reports. 

Adding non manufacturing time adds TAKT time. Added TAKT time = higher cost. 

That said, WIP = Inventory. Inventory = Money. Money = Taxation

Parts in inspection = WIP therefore there's a cost no matter where the part is within the factory. If you can integrate and automate processes you can bring down the labor component of part cost. 

"There are no perfect solutions, only compromises." Thomas Sowell

8 minutes ago, jas6142 said:

Support is the biggest concern with dmg without a doubt.

I hear that A LOT.

They like Yamazen use their AE departments as a training ground for the sales department... and it shows. Few of their AE's here in the US are dedicated to that craft for any REAL span of time. That's just the reality. I do know of an AE at Mori that's been with them since the 90's and I'd expect his to be a good 5-Axis guy since he came form Makino but he doesn't go out in the field... so what good is all that experience if you as a customer don't have access to it.

On 4/15/2024 at 11:30 AM, CEMENTHEAD said:

I would not recommend inspecting a part using the same machine that made said part. Been there, done that. 

It can be done effectively... it just has to be approached in the right manner.

The #1 issue with inspecting a part on the machine that produced it isn't that the machine is checking itself, it is that the connection between the coordinate system that manufactured the part and the coordinate system that is inspecting the part isn't broken. You MUST break that connection in order to get an accurate measurement.

On a 5-Axis machine with a FANUC control, that means having G68.2, G54.4, machine parameters set correctly, AND the probing software that supports probing with those functions active. Don;t have ALL those things squared away and there WILL be trouble in paradise.

1 hour ago, rgrin said:

...

Matsuura has been doing automated 5 axis forever.

...

Matsuura has been palletizing 5-Axis machines since 1992. They (as did the majority of 5-Axis builders) left that toilet bowl design the Germans seem hell bent on using in the dust LONG ago. It's not the best design for a table/table kinematic machine. Trunion is the best for table/table.

Support should be the #1 consideration when buying a 5-Axis machine. Much like a multi-tasking lathe support will make or break that machine. You could buy "the best" (whatever that is) machine but when the good for nothing AE shows up to train you, he (or she) has no clue about cutting parameters to utilize the machine to maximize it's capability, it's going to be on YOU to figure out. Oh sure, they'll tell you "... that's the CAM system's responsibility...", and it is, but only to a certain extent. When they cannot explain to you the role of point spacing, cut distance, and tolerance, and how it relates to machine performance, you ARE in for trouble.

https://schunk.com/us/en/workpiece-clamping-technology/manual-clamping-systems/c/PUB_8334 

www.raptorworkholding.com

https://www.mate.com/pages/metalheads/

To name a few...

When I need to do this I program a contour toolpath. On the filter tab I turn off arc filtering and turn on break arcs into line segments. I use CAMplete as my Post Processing solution and in there I change it from a 3+2 Toolpath to a 5-Axis (S-TCP) Toolpath then force it to either be on the correct side to keep it in travel. There are probably easier or other ways to do it, that's just how I do it. 

I just did a fresh install of CAMplete... Fusion360 was not installed automatically.

My understanding is the same as JP's... USB Hasp is a thing of the past. Relics of a bygone era. 

I haven't had one for quite some time. 

Legal; Neither me, nor my company are responsible for any paramters yiu change. Your machine is your responsibility.  It is advisable to consult a competent Machine Tool Applications Engineer that is familiar with your machine. 

Without further adieu, some of my favorites are as follows:

#929=1, 1=Always make FTP Data in  Attribute = ASCII

#1300.1 = 1 Handle Jog OT alarm not output. (NAL)
#1401.1 =1 No dogleg rapid (LRP)

#1401.4 = 1 Rapid Stops when Feed Override is at 0% (RF0)

#1604.0 = 0 AICC not on always in Auto Mode. (SHP)

#3106.6 = 0 During TWP or WSEC, "Absolute" position display is Program Coordinate system (DAK)

#3203.6 = 0 - Do Not Delete MDI  Program after execution (MER)
#3203.7 = 0 - MDI Program not cleared by reset (MCL)
#3204.6 = 1 - Do not Automatically erase MDI program. (MKP)

#3207.5 = 1 Display #500-#549 MACRO Variable Name (VRN)
7
#3233.1 = 1 (PDM) Folders in the Dataserver can be set as the foreground and background folder

#3301.7 = 1 Screen Capture Enable (HDC) - Hold Shift for 5 sec. 

#5004.2 - 1 = Diameter, 0 = Radius for CC. (ODI)

#5013 = MAX Wear Offset Value
#5014 = MAX INC Wear Offset Input (INP.+ Method)

#5148 (VMC Boring in Z-Axis)
Z 1 = Shift X+
  -1 = Shift X-
   2 = Shift Y+
  -2 = Shift Y-
ALL other axes = 0

#5200.5 = 1 High Speed style peck tap (PCP)
#5202.0 = 1 for Spindle Orient prior to rigid tap (reboot req.) (ORI)

#5213 = Rigid Tap Backoff Dist.

#5400.5 = 1 (LV3) Rotates MACRO Variables to be read in active coordinate system - For Probing in TWP.

#6001.3 = 1 Output all MACRO Variables on punch (PV5)

#6001.6 = 1 #100-#199 not cleared on reset. (CCV)

#6005.0 = 1 In Sub Program Call use Sequence Number (SQC)

#6008.3 = 1 On reset, POPEN is closed (KOP).

#6019.0 = 1 Output all variables as decimal number (MCO)

#6019.3 = 0 File Format of output file =PRNTnnnn.DAT (OFN) non =0000-9999

#6019.7 = 1 File Format of output file =PRNTnnnn.DAT (SFN) non =0000-9999 is memorized.

#11200.3 = 1 system variable #5061- #5080 Skip Coordinates can be read - for probing with WSEC active (WSK)

#11350.1=1 Current section of program only displayed, not look ahead section (APD) (Requires Reboot)

#11351.6=1 Parameter Group Names Displayed (GTD)

#13451.1 = 1 TWP 0's ok. (ATW)

#14701.5 & .4 = 1 Maximum clipboard size. (CLP) (Reboot Req.)

#14853.4 = 1 - Able to transfer from memory card to Dataserver. (Reboot Req.) (MDO)

#14854.6 = 1 Program Input/Output is enabled during Background Editing (BGO) 

#19746.4 = 1 (TBP) for G41.2/G42.2

So #19703-#19705 are your 1/2 offsets. Think of these as deviation from perfect alignment around the tilt axis and rotary axis intersections. The values for your table should have come with the paperwork for the rotary table inspection report.

Your machine should be a B/C kinematic so yiu would be concerned with #19704 and #19705.

An A/B would be concerned with #19703 and #19704, and an A/C machine would be concerned with #19703 and #19705. 

Unfortunately I'm away from my laptop today so I don't have all my info readily available. 

"Some" parameters are in maintenance books, some are in the connection manuals, others are in the Operation Manuals.common to Lathe Center.and Machining Center. It's a little confusing, but I kind of get it. 

I haven't found the descriptions to not be there. Some parameters are specific to builders and are not listed. 

3 hours ago, Seedy steve said:

IDK what that is... lol I am still learning g-code after 20 years!

this VCF has 3 meters of X , so if u r not close to position, it will often b out of range after g68.2 .

we r getting probing software Tuesday.

thanks again.

#5400.5 = 1 (LV3) Rotates MACRO Variables to be read in active coordinate system - For Probing while TWP is active.

Interesting about being out of range. In a few machines I've encountered over the years,  for some unexplainable reason, I've had to set #1301.7 = 0 Stroke Pre-Check Off because for some reason the control thinks it is going to overtravel while TWP was active. It's only been on certain  FANUV CNC Series and Edition Softwares. But the machine never did overtravel.  High Level Math... one of the great mysteries for me.

Interesting parameter differences.  

Why do you guys turn off LV3 off ever  @Paul Anderson? 

On 3/18/2024 at 6:05 AM, Seedy steve said:

I did need linear movement pre positioning to get within the range of motion for the offset/ angle. before g68 . (top mapped approach point)

I'm not familiar with top mapped approach point. 

I always have G54.4Pn in my code (Work Setting Error Compensation) which REQUIRES no linear position move until after G68.2

I missed you not having that function activated. My mistake.

There's different rules for different functions and different combinations of functions. 

As long as you understand what MockSim is and is not, what Vericut is and is not, what CAMplete is and is not you can make educated decisions about what fits your need.

MockSim doe NOT check G-Code. Tied to a Postability post it is a good solution for most things. Again, it's not fully simulating ALL the motion in your machine like M-Codes, etc...

Vericut... they simulate the actual G-Code that will run in your machine. As good as your control file and machine stuff is determines how good your simulation is. By and large it is the gold standard for simulation. You can create your own machines if you desire to learn or you can buy them from Vericut, or you can hire someone to build them for you. YOu have choices. Vericut is NOT an integrated post processing solution so you will need a post either from your CAM vendor or from ICAM, or somewhere else.

CAMplete... they simulate the G-Code created from their posted code. You cannot import and edited code. CAMplete IS an integrated Post Processing solution that will simulate the factory G and M-Codes. You have almost as much control over your machine as you would in a Vericut machine. You have limited machine editing capability and you cannot create your own machines. That is not an anticipated feature. The machines are factory configured meaning Matsuura, Okuma, Kern, Mazak, Haas, etc... has given their blessing on the accuracy of the models, motion, and functionality. Because CAMplete is an intagrated Post Processing solution, you have control over the code. The NC Formats are user customizable. Typically a basic NC Format is given to the customer that will run the machine well. I've got a decade and a half's experience developing NC Formats and I've got highly tuned NC Formats  that take advantage of the majority of the features and functions of the Matsuuras (since that95% of what I spend my time on) and I'm adding new stuff all the time based on customer requests.

Knowing the tools, knowing their strengths, weaknesses and capabilites os the key to getting the best solution for you. For me, nothing beats CAMplete. For you, Postability and Vericut may be best, for someone else, MockSim will do the job. Know your tools.