5 axis motion

[Mike Whitten CAD/CAM Contractors]

David,

 

I do not know why the machine is jerky as I have not seen that issue.

 

I found a good explanation of Inverse on the web. It explains it nicely:

 

Link

 

HTH,

Mike

[Mike Whitten CAD/CAM Contractors]

David,

 

There looks like there is a mistake in the second example above where they are getting F1400. It should be F140.

 

In simple form. If the machine travels 5" at 50ipm then it would take 5/50=.10 minute to complete. The inverse is 10 so F10.

 

It is easy to run this test. Just program something like a line and post it. I just did it. The code was programmed to .100" steps at 50ipm. .10"/50 = .002 minutes. The inverse is 500. The output from any of the posts around here was in fact F500.

 

Mike

[mcpgmr]

quote:

---

I do not know why the machine is jerky as I have not seen that issue

---

I had a part I was moving from a Matssura with an older Fanuc 11m to a Mazak H800 with M32 Control. It was X,Z,B motion using G93. Once I moved it the Mazak it alarmed out and wouldn't run. Seems the Mazak does not require the G93 because it knows that you are commanding a Linerar (IPM) and Rotary (DPM) at the same time and it calculates and times the motion automatically. But, The Mazak didn't have the processor speed and look ahead that the Fanuc had and the motion became very jerky. The jerkyness only caused dwell marks and didn't effect the part dimentions just caused some confusion on the floor.

 

As for programming gauge length. I found that it's ok if you are going to preset the tools and they are relatively the same each time you run the job. When I programmed this way I let the operator set up the tools and measure them with the presetter. He would them bring the gauge lenghts to me and I would plug them in and post from there. That tool list with preset values would be used everytime after that and if there was a case where a length had to be different because a tool holder was missing and had to be substituted, I would just re-post with the new tool length. Worked for me.

[dolphin1]

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?

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

do you have a way to turn on high speed machining.also keep the tilt and rotary un locked.this is what i have to do on the mazak i run.

[DavidB]

Thanks guys for the Inverse feed explainations.

 

I did a 50mm X 50mm square at 50mmmin feed rate and it posted G93 F1 so thats correct.

 

The machine alarmed soon as it read the G93. Illegal G code.

 

I looked at some old 5-axis programs that where done before my time in NCL.

code:

---

 N1421X-319.99Y200.536Z19.89F4200.0

N1422X-319.476Y200.714Z19.88

N1423X-319.108Y201.115Z19.859

N1424X-318.975Y201.642Z19.83

N1425Y203.428Z19.735

N1426X-319.141Y204.011Z19.704

N1427X-319.588Y204.42Z19.682

N1428X-320.184Y204.534Z19.676

N1429X-321.96Y204.379Z19.684

N1430X-322.474Y204.2Z19.694

N1431X-322.842Y203.799Z19.715

N1432X-322.975Y203.272Z19.743

N1433Y201.486Z19.839

N1434X-322.81Y200.904Z19.87

N1435X-322.362Y200.494Z19.892

N1436X-321.766Y200.38Z19.898

N1437X-287.697Y203.359Z19.739

N1438X-287.079Y203.305Z19.515A183.114B.057F2703.2

N1439X-286.538Y203.009Z19.308A183.163B.114

N1440X-286.0Y202.548Z18.831A183.273B.243F1427.0

N1441X-285.485Y202.109Z18.381A183.378B.365F1442.0

N1442X-284.921Y201.809Z18.177A183.435B.426F2620.3

N1443X-284.277Y201.77Z17.957A183.493B.486F2664.0

N1444X-283.451Y201.874Z17.968A183.508B.488F4200.0

N1445X-282.973Y202.05Z17.942A183.512B.493

N1446X-282.624Y202.421Z17.903A183.516B.498

N1447X-282.477Y202.909Z17.855A183.521B.503

N1448X-282.563Y203.413Z17.803A183.525B.508

N1449X-282.864Y203.826Z17.755A183.529B.513

N1450X-283.671Y204.512Z17.653A183.52B.521

N1451X-284.525Y204.769Z17.602A183.51B.525

N1452X-285.576Y204.643Z17.593A183.5B.523

N1453X-286.055Y204.468Z17.61A183.498B.521

N1454X-286.406Y204.098Z17.64A183.496B.518

N1455X-286.555Y203.61Z17.679A183.493B.515

N1456X-286.469Y203.107Z17.722A183.491B.512

N1457X-286.168Y202.694Z17.761A183.488B.51

N1458X-285.363Y202.006Z17.839A183.494B.505

N1459X-284.501Y201.75Z17.919A183.506B.497

N1460X-272.531Y203.285Z18.964A183.745B.341

N1461X-253.969Y205.867Z20.574A184.189B.085

N1462X-253.536Y205.928Z20.57A184.194B.086

N1463X-252.982Y206.108Z20.604A184.198B.077

N1464X-252.527Y206.469Z20.625A184.202B.067

N1465X-252.227Y206.966Z20.635A184.205B.058

N1466X-252.12Y207.535Z20.64A184.209B.048

N1467X-252.117Y207.881Z20.659B.038

N1468X-252.287Y208.477Z20.669A184.206B.025

N1469X-252.752Y208.885Z20.693A184.202B.012

N1470X-253.364Y208.976Z20.739A184.198B-.001

N1471X-254.14Y208.868Z20.744A184.192B-.002

N1472X-254.63Y208.675Z20.755A184.189

N1473X-254.977Y208.278Z20.78A184.186

N1474X-255.102Y207.766Z20.815A184.183

N1475Y206.977Z20.868B-.001

N1476X-254.928Y206.382Z20.913A184.189B.0

N1477X-254.458Y205.975Z20.944A184.194B.001

N1478X-253.842Y205.884Z20.951A184.199B.002

N1479X-253.066Y205.993A184.209B.003

N1480X-252.576Y206.205Z20.996A184.263B.004F3513.3

N1481X-252.229Y206.621Z21.03A184.317

N1482X-252.104Y207.152Z21.054A184.371

N1483Y209.846Z21.313A184.766B.0F2328.6

N1484Y213.568Z21.589A185.312F2326.2

N1485X-203.14Y220.589Z20.936F4200.0

N1486X-202.594Y220.77Z20.92

N1487X-202.147Y221.13Z20.886

N1488X-201.853Y221.622Z20.84

N1489X-201.751Y222.186Z20.788

N1490Y223.551Z20.661

N1491X-201.852Y224.011Z20.618

---

As you can see the above gcode does not have any G93 in it but it looks like it is using Inverese feed some of the time.? The only G codes in the whole program are G1 and G0. Some lines with X,Y,Z,A, and B have a feed rate and some don't. With Inverse a F value must be there on every line. So it beats me!

 

I get the impresion G93 does not need to be coded in.

I have rang the Makino rep twice its proving hard to get an answer.

 

The machine did come from Japan with the 5-axis rotary table so it should all be ready to go.

 

From the code above it looks like the machine can jump in and out of Inverse feed time without the relevant G codes? I ran a test program today and the machine alarmed with a G93 Illegal G code.

What do you think is happening with this code above?

 

Thanks all

 

[ 05-08-2007, 09:50 PM: Message edited by: DavidB@Rosebank-Engineering ]

[DavidB]

Ok guys this is what I have found out so far.

 

I ran a 5-axis swarf program of a 50mm square today and I found the following.

 

The machine can NOT eccept G93. Alarm Illegal G code.

 

The machine ran quickly and smothly with linear feeds in the program.

 

The same program with G05 P10000 (SGI) turned on made the Rotary motion very very jerky.

 

I have again contacted Makino and asked them if there is a special SGI for multi axis toolpaths.

 

Thank you very much to everyone who posted in this topic all the help is very much appreciated.

 

Is it worth asking the question how much $ to add the G93 option?

[DavidB]

For those that don't have the G93 option on there machines how do you run your multi axis toolpaths?

[mcpgmr]

quote:

---

For those that don't have the G93 option on there machines how do you run your multi axis toolpaths?

---

G94 most likeky. If your machine is a true 4 or 5 axis with a drive for each and G93 causes an alarm, I would assume that the control must have the ability to syncronize simultanious rotary and linear motion. At least that's what I experianced wuth the Mazak M32 as I mentioned earlier. Maybe there is another prep code?

[DavidB]

Guys I got quote from our Makino reseller.

Around $1500 to add G93 to our machine.

Would you go with it.

 

The machine does run smothly and quickly with 5-axis motion in linear movements.

 

Thanks

[Mike Whitten CAD/CAM Contractors]

I am unsure at this point. I think the question is "do you need it or not". I do not know the complete info on the machine but I do know some machines do not need it as Paul mentioned above. If you program the machine at a certain feedrate, does it appear that it goes that fast? Maybe have a look at the manual. Can the dealer supply sample multiaxis code?

 

Mike

[Bruce Caulley]

Personally, I would get it.

 

Bruce

[mcpgmr]

quote:

---

The machine does run smothly and quickly with 5-axis motion in linear movements.

---

I'm not so sure that G93 is the problem here. If your Rotary and Linear Axis's seem to be in time with eachother durng the machining but the motion is not smooth it may be just a memory buffer or look ahead issue. If this is not the case then yes I would invest the $$$ to have the G93 option turned on. Good luck! Keep us posted.

[DavidB]

Bruce,

Did you do any simultaneous 4-axis toolpaths on the A55's at your place of employment?

[DavidB]

Bruce-bump

[Bruce Caulley]

David,

No simultaneous on the makinos, but inverse feed made a HUGE difference to simultaneous 5 axis paths on the 3 mazaks.

 

One thing to check though is wether or not the c axis is locking after each move by default. We had that initially on the 2 variaxis and changed the default to unlocked and the toolpaths were immediately smoothed out.

 

Bruce