Well, I guess I'll chime in here a little bit.  For the question of if you can activate G43.4 H## without a z on a Fanuc 31i, absolutely.  Do it every day.  Not sure on our parameter setup, but there is no movement, but the absolute coordinates jump.  But we are on a head head machine.  Shouldn't make much difference going to a table table design, actually it likely makes it a bit easier.

99% of the time, unless I am up against a barrier, our format is:

G5.1 Q1 R#

G54

G43.4 H

G0 G90 X# Y#Z# B# C# S# M3

Basically speaking, I don't see any reason whatsoever if the machine doesn't move calling G43.4 H by itself in the current config.  If the coordinates shift when you execute that line, and it doesn't move, it is configured not to.  Then you can go about business as usual.

Now on another note, and I am by no means an expert on Table/Table machines, but why would one preposition with G68.2 then cancel and run TCP instead?  Seems confusing and cluttery.   In the example above using G68/G53.1, the post has already calculated and moved to the desired table angles, why call it again?  Is it just to make the machine and post are in agreement before you put a tool to the part?

Anyway.  Someday I hope to spend enough time on a table/table machines to understand some of these practices.  I have spent ooodles of time tinkering with approach and retract code on the head/head configs, and head/head/table (with TCP on head but not table), and if I had motivation, have notes of thoughts on post structures and methods that would be HUGELY useful for readability and general simplicity of adjustment at the control if one were focusing on short run work.   For the long run stuff it doesn't matter as much because you don't mind going back to CAM for quick edits, but when you are under the gun on a short run part, you just want to fix it in the program and move on.  Then catch the CAM up later when you are back in the office.  But someday I hope to have reason incorporate some really useful 5-axis features into a post.

I'm rambling again....  

IMHO, that's too much feed for Titanium to keep a straight hole and for the drill to hold up.

I'd be .0015-.002 ipr and about 110sfm, for best hole quality I would use a Kennametal YPL drill, three margin, acts like a gundrill.  For the cheapest thru coolant drill option I would use a Kennametal GOdrill.  Marginless, won't bind up in the hole, usually very good bang for the buck.

Sounds to me like you have a tuning issue (low likelihood) or hardware issue in the drive board to me.  If your Z-axis uses the same drive board as X or Y, you could consider swapping it with another axis and see if the problem goes away.  If that's the case then you have a bad drive.  There may be more sophisticated testing you could do.  But I am uninitiated in troubleshooting them by means of anything other than plug and chug.

Do you have more than one of these model machines to compare with?  If you feed it up in z slowly, stopping and starting frequently, is the load dead smooth and repeatable?  Unless you have a right angle head, you can't really easily do a test that would repeat an issue I once had.  But if you side mill while compound feeding that axis with another while it is loaded (Z+) , you would be able to see it clear as day in the finish.

What does the load look like while it is cutting?  Does it fluctuate greatly?  Maybe the inertia parameter isn't set right and happens to react with that harmonic?  Have you tried faster or slower spindle speeds with success?

11775.0 is Smooth TCP correct?  It would seem to me that it isn't configured properly on the machines that don't like it......

That would be a fun one to dive into and diagnose.  But also goes to show how all of those options intertwine and make it very hard to configure a "stock" configuration, that works on most setups.  No two builders option machines exactly the same, no builder typically options two like machines exactly the same either....  That to me is the head scratch.

On 8/14/2023 at 12:21 PM, crazy^millman said:

Testing and seeing where the best ROI gives is what really needs to be done.

DING DING DING

When running high feed cutters, in my experience, when climb should have worked best, conventional cutting has worked better, as well as the opposite case.  It is highly dependent on toolpath style as well as material and part shape.  When running in Ti, Inco, or other super alloys, I now always advise my customers to try both ways.  I have seen 3-5x differences in tool life with zero difference in processing time or speeds and feeds.  When you get that much more life often I have been able to really boost productivity by then balancing the tool life with speed and hitting the right tool change interval.  Let's just say you get 1 part going climb, you switch to conventional and you get 5 parts.  You then increase the speed 30%, and now you get 2.5 parts.  So you bump it up 5% more and now you get 2.1 parts and change them at 2 so you have a little wiggle room.  35% on productivity is huge and think, you are using 50% of the inserts you were.  It's a made up example, but to Ron's point.  TEST TEST TEST, you won't know unless you try.

Another thing to note when you have some inserts that are worn and others that don't appear to be.  Runout is certainly the normal cause.  Fix that and the problem will be less apparent.  But I find usually it is also a sign that you don't have the right cutting parameters.  If you are taking enough chip load and are going fast enough to not get built up edge a few thousands of runout won't cause you any harm.  But if going too slow, some inserts may be failing early due to built up edge ripping the coating off the inserts.  This will appear randomly as wear on some inserts but not on others especially on easy to machine softer steels like A36.  Otherwise, too little feed will rub on some and cut on others as the difference in chip load due to runout will put you on the other side of not enough feed.  Feed 25% harder and it might go away.  If it doesn't, check the speed.  If it were me...  In A36, I would be running a CVD coated insert @1200+ SFM and about .010"ipt as a starting point.

Unless you have ground inserts, .0005" runout axially or radially is asking for a bit much.  For standard pressed inserts in a milling cutter .0015-.002 isn't abnormal, especially in the 3-5" range.  If the inserts are clocked the same way they were pressed, .001 should be achievable, but you may have to play with swapping inserts and pockets around, or custom clocking the inserts to fine adjust, especially if there is a little mileage on the cutter.  For ground periphery sub .001, should be pretty easy as long as everything is clean, and the body and mounting is in good shape.  If your screws are worn, replace them, so you can get consistent torque.  Better yet torque your screws, and plan to replace screws on a regular basis.

16 hours ago, David Colin said:

To be able to edit 3D tools components, plane manager needs to be docked with settings panel.

Boy that is an annoying bug.  But at least someone has figured that out!

On 3/28/2023 at 11:05 AM, ?Mark said:

While we're on this topic....does anyone have some Microsoft 3.11 era computers laying around in the attic somewhere?

I just disposed of one last year.  Bummer.  Doubtful, but there still might be one at my parents place.  The one I have in mind was an IBM with 8MB of RAM.  Was an expensive one back in the day.

On 4/14/2023 at 4:23 PM, SlaveCam said:

Shouldn't G54.2 be the easiest of all? "Many" use it with mcam without any post modifications (from what I've read on different forums), as the work offset simply rotates with every B-command and all you have to do in mcam is rotate the plane (origin stays in place).

Anyways, I've been experimenting G54.2 on SmoothG control and already losing my patience. Why does G54.2 perform axis motion?? Is it same on Fanuc or another Mazatrol idiocy?

 

I believe G54.2 on a Mazatrol is more akin to G43.4 on a Fanuc.  That is old corrupted memory..., but as I recall that's the case.

On 4/7/2023 at 2:16 PM, Aaron Eberhard said:

I put that <stuff> on EEEVVEEERRRYYTHING.

Happy I'm not the only one 

I pretty much do all of my surfacing with morph or parallel strategies now.  Once I got to know how to manipulate them, I just don't want to use the standard 3D toolpaths anymore.  The only time I really do use the standard 3d paths now is when I need cleaner "filtered" code due to memory or control constraints, or I am helping a customer that doesn't have Multiaxis in Mastercam. 

I have had to do this with patterning as well in the past for making parts on multiple faces.  You will end up with crapload of transform operations, but it is absolutely possible to do it with sub programs, and also possible to maintain 100% associativity back to the main operations.   You can have it wind up and unwind your rotary as you go tool by tool as well.  Makes for a very efficient executing program with fewest tool changes and least amount of rotary movement.  Lot's to keep track of, but at the end of the day it works very well.  IIRC to rotate 180 degress in xy and then 90 about y, then pattern with work offsets, and sub, it took 4 or 5 transform ops to do it properly.  Also, the mention of going crosseyed is also a very mild description of what happens if you walk away and try to come back and decode what you have to do to alter/finish the job.

9 minutes ago, mirek1017 said:

and I need to set up part 3 inch high ,so how I should programing z on mastercam

XYZ zero will be at COR, and offset will match same location in the machine  If there is an offset between the two rotaries, you will need to put that in the post.  Should be a pretty small value in this case.

Does your IT Department manage the pc's using an image?  Or if they do manage them with scripted installs, you could theoretically script the installs and then make a quick powershell script that would copy all needed files to each machine.  That said, do it with JP's method and just push the config file out to each machine once it is installed.

On 9/6/2022 at 8:52 PM, gcode said:

 

Safe Index forces a Z retract before X and Y motion

In my recollection, all safe index does is split the xy and rotatry motion onto two lines.  The Z retract is only affected by ret_on_index.

But it's been a while since I played with or modified that logic, I have made heavy modifications to this logic many times, more than I should have for sure, so I may be mistaken on that.

Yeah I have a had this idea to control high speed settings (G05.1 ect), for a while now.  Haven't done it yet, but I will eventually.  For me I would use it on top of MI/MR values and make it so you can do one or the other.  One of those things that you need to know it's there to use it.  Hence why it likely isn't done very often.  but being able to use comments to pass data, you can pass a lot of settings in a very efficient manner when it comes to turning them on and off.

Upload a zip to go with your post in it, or shoot me a pm and I'd be glad to take a look at it.

I think everyone zipped past it.  But if you read the code the first feed move is actually the arc move, it should be the first Z move where the F25. is called out (missing a G01).  My bet is it is actually a post issue, nothing to do with his mcam file.  The null toolchange position line likely isn't updating gcode to 0 likely commented in with "" and therefore modality thinks it is in G1 already... which it isn't.  Hence when the value changes to 3 for the first arc move it outputs a G03.  Does it do this any time you have two operations in a row with the same tool?  Quick fix/test would be to check the force tool change on the tool page and see if the behavior is corrected when coming in from a fresh "toolchange".

IMHO, Using a macro variable to check for the right condition during execution is the best way.  This is easily be accomplished through some post mods.

Basically, when you do a tool change check to make sure the offsets are setup correctly for how you have it programmed.

So if that program is in the wear convention you will have the post output a check at each tool change to make sure the offset values are programmed to the expected magnitude, 10% of the tool diameter is usually more than enough. 

You could also do it at the operation level in Mastercam and throw an alarm during cutting execution, and check to see how comp is set for that op at both the tool change and null tool change portions between ops.

Many different options here.

G10's are fine, but then you would have to add them to all of the programs from the past to make sure those are correct, when you run a legacy program.

Theoretically you could hit the flats, but you will never get the corners with a 4 axis swarf cut.  That said, you could cut the flats and then surface the corners.  You wouldn't even need swarf to at all do it that way either.  You do it 3+1.

Happy grammin'

With A286 you are in the realm of needing to make a chip but not rub like any other S3 type Nickel based material.  As mentioned earlier, runout is killer with these small tools as usually runout is easily greater than your chipload...   

Just as a rule of thumb, it is pointless to run a chipload less than your runout...  I have found that chiploads under .0002" usually don't have any benefit any typically yield worse results with anything larger than .062", but given your cutter diameter, you will need to reduce some if slotting, so their recommendation of .0001" should be achievable, but you will have to have runout less than half of that likely, and you will need to find a sweet spot where you can still make a chip, but not overload the cutter and break it from bending load.

SFM likely won't matter much as you probably don't have enough spindle speed to actually burn up a cutter, and is more going to be a function of balance and how dynamically stable your spindle is.

10 hours ago, TerjeS said:

but the bosses aren't too keen on such a large investment into training and software licences, PC's or servers capable of running it, and all the previous programs that would have to be re-made.

How often do you need these complicated subs?  If it is all the time then maybe you need all of the above.  But if it is just a once in a while, then it shouldn't be an issue.  You would only run that entire part in EIA, you wouldn't have to ditch Mazatrol for the simple parts.

Any chance you can call a Mazatrol program from an EIA program?

On 7/15/2022 at 5:22 PM, crazy^millman said:

Highfeed style cutter would be ideal for this.

For Finishing?   Depending, I guess it could be done, but it is going to push on the plate more than a 45degree cutter will.

I would say a positive positive (positive insert, positive axial/radial rake) style 45 degree facemill will be your best bet.

Kennametal KSOM Mini cutter (KSOM200OF5345M3) with OFKT53AFEN6LB inserts in KC522M grade would be pretty hard to beat.

Otherwise, a Dodeka Mini would be a possible good choice with ground periphery (HNGJ) and LD chipbreaker inserts in KCSM40 grade, it just won't be quite as free cutting as the KSOM.

Both would be very versatile, as there are many insert choices to choose from if needed.

Can someone explain to me why a three point Adjustable jaw boring ring needs to be accurate?  IMHO there is no way the counter bores in soft jaws are held to that tight of a concentricity/runout tolerance, which would defeat the purpose of an accurate boring ring.  Nice fits to the jaw counterbores would be a nice to have, but once again, I don't think it's needed.  What's most important is that when you spin the ring to open it into the correct location, that it's close enough and won't bind sideways between two jaw, but instead pushes to the center.  If it's pushing to the center the forces will be properly balanced between the jaw, they have to as it needs to form an equilibrium.

Ready to be edumacated here. 

On 6/10/2022 at 7:29 PM, srbeyke said:

but I really don't think that

step up cutting will work in my application

Then you will need to create multiple Optirough paths with each step as the max depth top to bottom.

But I believe Ron is correct, step up would be the way to hit the other flats automagically.  Otherwise, your step down would need to hit each step evenly for it to clean each step with the same stock as you go down.  I "think" if you have a small step down, and a "large" step up (say 1/2 of the step down) it will hit those flats at your stock allowance, and won't add a bunch of extra passes.