5 axis motion

[DavidB]

I just posted my first 5-axis simultaneous toolpaths.

I have a few qustions.

 

The machine (Makino A66 Pro3) alarmed with G05 P10000 (SGI) with these toolpaths.

I would have thought this would have helped as there are lots of point to point moves, each line has an XY A and B move. I could not find in the manual that 5-axis simultaneous moves could not work under SGI. When I removed the G05 P10000 the machine ran fine.

 

The second is should multi axis toolpaths use inverse feed over linear feed rates?

I'm using the Generic Fanuc 5-axis post.

 

Thanks

[Greg Williams]

David,

 

It is best to use Inverse time feed when working with toolpaths that contain rotary moves. As for the HPCC thing I am no Makino expert but it sounds like you don't have that option

[DavidB]

Greg,

Is it much work to the post to setup Inverse feed for simaltaneous toolpaths only?

[gcode]

There is a switch in the generic 5X post

to enable inverse time.

The machine definition also has this switch, but

I don't think its functional yet.

With inverse time, the bigger the F, the slower the feed rate.

Find out if your machine will accept 4 digit feed rates. The post defaults to F999. as the minimum

output. If your machine will accept it, change that to F9999.

 

This is the section of the X2 generic 5X post

where you set feedrates

 

[*]#Feed control settings

convert_rpd$ : 0 #Convert rapid to rapid feed

use_fr : 0 #Output feedrate

#0 - programmed feedrate

#1 - inverse feedrate

#2 - inverse feedrate on 5 axis continuous

#3 - inverse feedrate on motion with rotary

inv_fd_typ : 0 #Calculate feed location options

#0 - inverse feed at tip

#1 - min-max on flute length

#2 - tip to pivot on tool length

#3 - min-max on flute length to pivot on tool length

inv_sec : 0 #Inverse feedrate is in seconds

radius_fr : 0 #Use axis radius distance (pri_feed, sec_feed), user must add code

rot_feed : 0 #Rapid rotary motion only feed options

#0 - convert to G0 rapid

#1 - apply rapid feedrate

maxfeedpm : 500 #Limit for feed in inch/min

maxfeedpm_m : 10000 #Limit for feed in mm/min

maxfrinv : 999.99#Limit for feed inverse time

fix_fr : 1 #If feedrate is zero, apply these values

deffeedpm : 1. #Default for zero feed in inch/min

deffeedpm_m : 25. #Default for zero feed in mm/min

deffrinv : 500. #Default for zero feed inverse time

[Mike Whitten CAD/CAM Contractors]

David,

 

As I remember, Makino had a seperate M-code modifier for multi-axis code when using SGI. Maybe is was M254 or something like that. You may need the actual SGI booklet to find this info though.

 

Mike

[john316]

.

 

The Gen5x post will switch from inverse to linear by itself when you set it up for inverse feed. The codes are G94 for linear and G93 for inverse. When you post you will see those in your nc code. The inverse will also have a feed on every line.

 

.

[Greg Williams]

quote:

---

With inverse time, the bigger the F, the slower the feed rate.

---

I think it is the other way around.

[DavidB]

Mike, I have the SGI booklet at work, the toolpaths I posted where not in Inverse feed time.

 

Would this be why G05 P10000 caused an alarm?

Maybe it needs Inverse feed for mutli axis movement?

 

Monday at work I'll set the post up for Inverse feed and see If I can use the SGI.

 

Thanks guys

[Mike Whitten CAD/CAM Contractors]

It is hard to say what caused the alarm. I have never tried any multiaxis milling without inverse feed.

 

I think if you turn inverse feed on and maybe play with SGI a little, you should be good to go.

 

Mike

[Greg Williams]

David,

 

I think you may find that Inverse time Feed is also an option for your machine you may need to contact Mr Makino.

 

Your code should look something like this, You may or may not need the M codes

 

X-8.157 Y-78.727

Z207.865

Z172.865

G1 Z157.865 F1000.

G93 X-8.872 Y-77.418 Z158.351 A-65.5626 C93.5104 M115 F2967.5

 

X-10.291 Y-74.862 Z159.258 A-64.7186 C93.5158 M115 F1505.2

 

X-11.545 Y-72.648 Z160. A-63.9862 C93.5162 M115 F1715.8

 

X-12.94 Y-70.233 Z160.765 A-63.1855 C93.512 M116 F1552.5

 

X-14.39 Y-67.776 Z161.494 A-62.3683 C93.5035 M116 F1502.5

 

X-15.777 Y-65.472 Z162.131 A-61.5996 C93.492 M116 F1577.

 

X-17.244 Y-63.084 Z162.744 A-60.8003 C93.4768 M116 F1496.7

 

X-18.556 Y-60.99 Z163.239 A-60.0962 C93.4614 M116 F1676.6

 

X-19.993 Y-58.74 Z163.728 A-59.3369 C93.4428 M116 F1533.7

 

X-21.476 Y-56.461 Z164.176 A-58.564 C93.4224 M116 F1484.7

 

X-22.789 Y-54.481 Z164.525 A-57.8895 C93.4041 M116 F1676.4

[Mike Whitten CAD/CAM Contractors]

quote:

---

I think you may find that Inverse time Feed is also an option for your machine you may need to contact Mr Makino

---

This has happened to me. It is very unfortunate that the dealer will sell a multiaxis machine and not suggest to the customer that they should purchase the option. For that matter, what would one do without it?

 

Mike

[DavidB]

Post mod:

 

code:

---

 #Feed control settings

convert_rpd$ : 0 #Convert rapid to rapid feed

use_fr : 0 #Output feedrate

#0 - programmed feedrate

#1 - inverse feedrate

#2 - inverse feedrate on 5 axis continuous

#3 - inverse feedrate on motion with rotary

inv_fd_typ : 0 #Calculate feed location options

#0 - inverse feed at tip

#1 - min-max on flute length

#2 - tip to pivot on tool length

#3 - min-max on flute length to pivot on tool length

inv_sec : 0 #Inverse feedrate is in seconds

radius_fr : 0 #Use axis radius distance (pri_feed, sec_feed), user must add code

rot_feed : 0 #Rapid rotary motion only feed options

---

Can someone guide me through the settings please?

use_fr should it be 2 or 3?

inv_fd_type should it be 0 1 2 or 3?

inv_sec ?

rot_feed ?

 

Thanks

[DavidB]

Code now looks like this.

code:

---

 N8301

G21

G0 G17 G40 G80 G90 G94

G91 G28 Z0.

M11(UNLOCK-

M13(UNLOCK-A)

( 16 X R2 TOOL - 83 DIA. - 16. )

( CLEVIS SHAPE 5-AXIS TOOLPATH )

T83 M6

M97

M56 H1 D2

G0 G54 G90 X-205.169 Y47.187 A99.704 B1.897 S1600 M3

G43 H1 Z88.717

G05 P10000

M8

G1 G93 Z68.717 F50.

X-204.754 Y45.822 F700.88

X-204.148 Y44.53 F700.88

X-203.365 Y43.337 F700.88

X-202.42 Y42.268 F700.88

X-201.333 Y41.344 F700.88

X-200.125 Y40.585 F700.88

X-198.821 Y40.005 F700.88

X-197.448 Y39.617 F700.88

X-196.034 Y39.428 F700.88

X-194.607 Y39.442 F700.88

X-193.197 Y39.659 F700.88

X-191.185 Y40.088 Z70.347 A99.789 B1.389 F349.7

X-189.14 Y40.41 Z71.989 A99.848 B.877 F349.7

X-187.067 Y40.624 Z73.64 A99.88 B.363 F349.7

X-184.972 Y40.731 Z75.293 A99.886 B-.152 F349.7

X-182.858 Y40.729 Z76.945 A99.865 B-.666 F349.7

X-180.733 Y40.618 Z78.592 A99.818 B-1.179 F349.7

X-178.6 Y40.4 Z80.228 A99.744 B-1.689 F349.7

---

The machine did NOT alarm with G93 and SGI.

 

The problem now is the machine using G93 is very jerky it is not smooth like it was when I was not using Inverese feed?

The rotary motion is jerky?

[DavidB]

Is the feed rate normally in minutes or seconds?

inv_sec : 0 #Inverse feedrate is in seconds

 

Because my 5-axis for this machine is a rotary rotary that goes into the machine I can't find any info or manuals at work on it.

 

inv_sec : 1 #Inverse feedrate is in seconds

Gave a feed rate to slow to be corrcet so I assume its in minutes.

The machine is very jerky though the only differance in smotth code and jerky code is the G93 if I ran the same toolpath with a G94 it cuts nicely.

Any ideas?

[DavidB]

In the operation manual.

M250 GI,super GI standard mode

M251 GI,Super GI quick mode

M252 GI,Super GI hidh-precision mode

M253 GI,Super GI special mode

M254 GI,Super GI M254 mode

M255 GI,Super GI M255 mode

 

Anyone know anything about these M codes?

[Mike Whitten CAD/CAM Contractors]

David,

 

I am not a post guy but until better/other info comes along here goes:

quote:

---

Can someone guide me through the settings please?

use_fr should it be 2 or 3?

inv_fd_type should it be 0 1 2 or 3?

inv_sec ?

rot_feed ?

---

I would set the "use_fr" to 3 I believe this just means to use Inverse on any type of rotary(5ax code) motion. I have a post that I have used and one that I believe to be good that has it set that way.

 

"inv_fd_type" I always leave this set to 0 only because I don't know any better. There may be special machines/situations that require different though.

 

"inv_sec" I have only used and seen this set to 0

Here is a clip from the Haas website.

 

-------------------------------

Inverse Time Feed Mode (G93)

This VMC/HMC feature specifies that all F (feedrate) values are to be interpreted as “strokes per minute.” This is equivalent to saying that the F code value, when DIVIDED INTO 60, is the number of seconds that the motion should take to complete. G93 is generally used in 5-axis work, and sometimes in 4-axis work as well. It’s a way of translating the linear (inches/min) feedrate assigned to the program – F30, say – into a value that takes rotary motion into account. When G93 is activated, the F value will tell you how many times per minute the stroke (tool move) can be repeated, based on the linear F value.

 

Haas has been able to accommodate full 5-axis machining for many years; however, this feature, in conjunction with aftermarket CAM systems and their post-processors, offers even more flexibility and versatility.

-----------------------------

 

"rot_feed" I have only used and seen this set to 0. I believe this just means convert the NCI rapid to rapid feedrate instead of G0

 

 

quote:

---

The machine did NOT alarm with G93 and SGI.

 

The problem now is the machine using G93 is very jerky it is not smooth like it was when I was not using Inverese feed?

The rotary motion is jerky?

---

Is this with "use_fr" =3 ?

 

 

quote:

---

In the operation manual.

M250 GI,super GI standard mode

M251 GI,Super GI quick mode

M252 GI,Super GI hidh-precision mode

M253 GI,Super GI special mode

M254 GI,Super GI M254 mode

M255 GI,Super GI M255 mode

 

Anyone know anything about these M codes?

---

The Makinos I dealt with were a bit older. 1994-1998 models so that is what the following info regards.

 

Makino just assigns different parameter sets in the control for the acceleration and deceleration type settings. Back then, all the machines we saw had very conservative settings that would drive a guy nuts unless you were not in a hurry. We had the Makino enginneers work up some special settings to induce a specific inaccuracy for each M code. IOW, we had standard mode, quick mode and "supersonic". We actually had them loosen up the settings so much so as to allow a .004in inaccuracy for the rough mode(supersonic. This would allow 1000ipm feedrates in 2d and 300-500 in 3d without slowing down. As I remember you just code like this:

 

M251

G05 P10000

 

There is probably more advanced High Speed stuff nowadays but I am not to up on it.

 

HTH,

Mike

[DavidB]

This is an example of the gcode that is jeky and has Inverse feed time.

use_fr : 2

code:

---

 G1 G93 Z68.717 F50.

X-204.754 Y45.822 F700.88

X-204.148 Y44.53 F700.88

X-203.365 Y43.337 F700.88

X-202.42 Y42.268 F700.88

X-201.333 Y41.344 F700.88

X-200.125 Y40.585 F700.88

X-198.821 Y40.005 F700.88

X-197.448 Y39.617 F700.88

X-196.034 Y39.428 F700.88

X-194.607 Y39.442 F700.88

X-193.197 Y39.659 F700.88

X-191.185 Y40.088 Z70.347 A99.789 B1.389 F349.7

X-189.14 Y40.41 Z71.989 A99.848 B.877 F349.7

X-187.067 Y40.624 Z73.64 A99.88 B.363 F349.7

---

This is the same toolpath posted with linear moves G94 and runs smoothly.

code:

---

G1 Z68.717 F1000.

X-204.754 Y45.822

X-204.148 Y44.53

X-203.365 Y43.337

X-202.42 Y42.268

X-201.333 Y41.344

X-200.125 Y40.585

X-198.821 Y40.005

X-197.448 Y39.617

X-196.034 Y39.428

X-194.607 Y39.442

X-193.197 Y39.659

X-191.185 Y40.088 Z70.347 A99.789 B1.389 F500.

X-189.14 Y40.41 Z71.989 A99.848 B.877

X-187.067 Y40.624 Z73.64 A99.88 B.363

---

The only differance is the feeds, so I asume the feed is making the machine jerky?

I rang Makino to find out about the M-codes and I'm waitng for a reply.

 

Thanks Mike

[MLS]

David,

 

I believe the Pro3 has the capability to run in G43.4 which eliminates the need for inverse time feedrate. Don't know if it would be compatible with that machine, but another possible option.

 

Might ask your Makino rep about it.

[DavidB]

G43.4? That's for tool length is'n it?

 

How does MC come up with an Inverse feed rate of F349.7 for a 500mmmin linear feed rate?

[MLS]

Yeah David.

 

G43 is a 3-axis tool length comp

G43.1 is a 5-axis tool length comp

.

.

G43.4 is a tool length comp that also calculates for pivot distance so it can track the tip and apply a linear feedrate to the tip of the tool.

 

I.E. No G93 required because the control figures it all for you and feeds the tip at your linear feedrate.

[Mike Whitten CAD/CAM Contractors]

David,

 

quote:

---

How does MC come up with an Inverse feed rate of F349.7 for a 500mmmin linear feed rate?

---

The clip I posted above says how. I pulled it from the Haas website. The fanuc book should also have an explaination.

 

 

MLS,

 

This G43.4 sounds cool. I will check that one out.

 

Thanks,

 

Mike

[crazy^millman]

G43.4 would be the only way I would program the machine.

 

The thing you need to think about is you are programing to a gauge length and need to maintain that gauge length everytime you set-up and run that job. If you do not have the operator maintain that then you are going to have tolerance and accuracy issues with your parts. If you let the machine do the dynamic compensation now you program all of your tools like a standard 3 axis part. The other advantage depending on how the machine handles tool offsets is that you can easily switch between 3 axis and 5 axis toolpaths in the same program with the same tool and have all of the numbers make sense to the people running the machine. The thing you find if you always program gauge length is you will always be reposting programs and always running the rick of scrapping part.

[MLS]

+1 Ron

 

It has been so long since I have posted with a gauge length I didn't think of that.

 

I am wondering now if you do post it with a gauge length, won't that cause an inaccuracy in the calculation of the feedrate?

 

The control has to know the tool length offset in addition to the pivot distance to accurately calculate it.

 

We always program to tip of the tool, but I don't really know if you have to or not.

 

[DavidB]

Thanks for the help guys.

 

Going back a step why would the machine be jerky with Inverse feed and the feed rates in the program posted above, but ran smoothly with linear feeds?

 

 

quote:

---

Inverse Time Feed Mode (G93)

This VMC/HMC feature specifies that all F (feedrate) values are to be interpreted as “strokes per minute.” This is equivalent to saying that the F code value, when DIVIDED INTO 60, is the number of seconds that the motion should take to complete.

---

So I take G93 F349.7/60=5.82 seconds to complete a line of code.

[Greg Williams]

David,

 

Like this

 

G93

G1X100S100M3F0.5 The block is executed in 2 minutes.

G1X50Y50Z100S100M3F6 The block is executed in 10 seconds.

G3X50Z50I50 K0S100M3F1 In the circular interpolation mode, feedrate is determined

according to the arc radius as explained above.

(FRN = Feedrate / Arc radius)