Mazak new SmoothX control

[jlw™]

Started making chips in our new E1600 today.

 

Any one else running a smooth controlled mazak?

 

It has some wicked awesome stuff in it. My two favorites are stock recognition and trochoid milling.

 

Yes! Stock recognition in the conversational! Start with a turning op, move to a tilted plane and make a couple milling paths, they acknowledge stock!

 

Trochoid milling is not new but it's nice to have in mazatrol because I simply hate burying a tool.

 

A lot of copy/paste stuff in the programming and in the offsets screens.

 

I'm digging it!

[Zoffen]

How is using the onscreen keyboard and keypad?

 

I have used some of the demo controls and really dislike not having a physical keypad to key in values with.

 

The Highspeed milling in mazatrol is sweet! We are an all mazak shop with lots of simple mazatrols parts that the guys on the floor program. It would be great for them to be able to program sweet roughing paths instead of bothering me!

 

Did you get the spec on the new encoders they use. They have a crazy amount of steps per rev its nutz!

[jlw™]

We do a lot of mazatrol as well.

 

We're exclusively mazak as well except for one loner haas, a bridgeport and two manual lathes we do some hardcore roughing on.

 

I was a little irritated at not having a keyboard at first but it's actually a little more intuitive than you might think.  The HMI is a windows 8 box so you can swipe left on the right side and click the keyboard any time you want.  Once you find all of the buttons it's pretty nice.  I've only had my hands on it for a couple days and maybe a total of about 2 hours on the panel.  I loaded up about 80 tools and played with the probe a bit.  We started making some risers for our chuck jaws and they will actually be the first part but I drew and programmed it in mcam.  It looks to be very promising!  The only trouble I've had is manipulating the views.  You can now pan/rotate the toolpath and 3d machine screens like a tablet or phone and it's quirky but THEY ADDED A FIT BUTTON TO TOOLPATH!!!

 

Mazak hit it out of the park in my opinion.

[Newbeeee™]

Fanuc has trochoidal machining.

Providing you load a mastercam file into it....lol

 

What's with all this on-machine programming?

Not very cost-effective.

 

/tin hat off

[m98custom1212]

Fanuc has trochoidal machining.

Providing you load a mastercam file into it....lol

 

What's with all this on-machine programming?

Not very cost-effective.

 

/tin hat off

Because some stuff donesn't require mastercam.. the operator or foreman can quickly program a job.. fixtures.. quick easy job that comes though don't have to bother a programmer that is working on something else... endless things

[jlw™]

Because some stuff donesn't require mastercam.. the operator or foreman can quickly program a job.. fixtures.. quick easy job that comes though don't have to bother a programmer that is working on something else... endless things

Ditto.

 

If something needs one face cut a fuzz deeper or one hole popped it could be done at the panel faster than they can bring me the packet.

 

It has its place.

[Newbeeee™]

 

How many more???

[Pitka_Guru]

Hi Guys, 

 

Interesting timing of this thread as we have just received our first Variaxis i600 Smoothx and a 6 pallet changer. We have X9 with Postability's Variaxis post. We run ISO only and are having issues with feedrates, jerky cutting motion and tool breakages.

 

We can run ~400ipm (10M/min) and have tried G05 P2, with G61.1 and using the M820-M830 options. I'm sure we are doing something wrong with these settings or we need to dig further into the controller's parameters?

 

Can anyone offer some advice on how to achieve higher and smoother feeds?  Unfortunately the Mazak techs in this hemisphere are not very helpful with 5 axis or ISO. 

 

Cheers

[jlw™]

Can you send me an mcam file and your posted program?

[Pitka_Guru]

Yes, I can post some of the code here and I'll see if I can get the mcam file from our server to send. Thanks heaps

[So not a Guru]

Hi Guys, 

 

Interesting timing of this thread as we have just received our first Variaxis i600 Smoothx and a 6 pallet changer. We have X9 with Postability's Variaxis post. We run ISO only and are having issues with feedrates, jerky cutting motion and tool breakages.

 

We can run ~400ipm (10M/min) and have tried G05 P2, with G61.1 and using the M820-M830 options. I'm sure we are doing something wrong with these settings or we need to dig further into the controller's parameters?

 

Can anyone offer some advice on how to achieve higher and smoother feeds?  Unfortunately the Mazak techs in this hemisphere are not very helpful with 5 axis or ISO. 

 

Cheers

 

Have you had any problems with 5-axis toolpaths? We just got a Variaxis i800 & we also have the Postability post.

The 1st 5-axis path we ran today went completely awry, and scrapped a par.

I suspect that the machine parameters are set incorrectly, unfortunately we have the same trouble with our Mazak reps.

 

Zeke

[jlw™]

Have you had any problems with 5-axis toolpaths? We just got a Variaxis i800 & we also have the Postability post.

The 1st 5-axis path we ran today went completely awry, and scrapped a par.

I suspect that the machine parameters are set incorrectly, unfortunately we have the same trouble with our Mazak reps.

 

Zeke

 

 

Yep, same trouble.

 

How are you handling tilted planes?  Parameters depend on that.

[Zoffen]

How are you doin 5 axis stuff? G43.4? Did you change the parameter that deals with locking the coordinate system to the table?

[jlw™]

for full 5 we use G54.4/G43.4 set by MI.

 

For all 3+2 I use G68 or G68.2 and I have 3 Postability posts.

 

Send me a pm.

[So not a Guru]

How are you doin 5 axis stuff? G43.4? Did you change the parameter that deals with locking the coordinate system to the table?

We just got the correct parameters that should be set, from our Postability reseller, today (after spending the last 3 weeks trying to get the info from Mazak, postability got it to us in one day). We actually have a Mazak applications engineer coming tomorrow morning to see if they can get this darned thing to work.

 

Zeke

[Colin Gilchrist]

We just got the correct parameters that should be set, from our Postability reseller, today (after spending the last 3 weeks trying to get the info from Mazak, postability got it to us in one day). We actually have a Mazak applications engineer coming tomorrow morning to see if they can get this darned thing to work.

 

Zeke

 Could you please post up the list of parameters, and the "expected" values for the Postability Posts to function correctly?

[So not a Guru]

 Could you please post up the list of parameters, and the "expected" values for the Postability Posts to function correctly?

F3: set to 1

F36:00000110

F85:00011000

F86:01100100

F91:00010000

F92:10101000

F93:00001000

F96:01000000

 

These are the settings we were given, they are dependent upon:

 

tcp          : 2     #Enable tool center point management

tiltplane   : 1     #Enable tilted work planes

 

being set in your post.

 

Zeke

[So not a Guru]

Keep in mind that we have not had the opportunity to test this yet. Hopefully tomorrow.

[JMahon]

Repost

[JMahon]

for full 5 we use G54.4/G43.4 set by MI.

 

For all 3+2 I use G68 or G68.2 and I have 3 Postability posts.

 

Send me a pm.

 

On mazaks, is posting G68 in EIA like using wpc shift and index mazatrol?

 

That sounds very useful to us. We have a sort of hybrid programming style where I work. Some guys do all 2d in mazatrol and post the 3d from mastercam. The rest use center of rotation 100% from mastercam.

It would be much easier on the operators.

[jlw™]

On mazaks, is posting G68 in EIA like using wpc shift and index mazatrol?That sounds very useful to us. We have a sort of hybrid programming style where I work. Some guys do all 2d in mazatrol and post the 3d from mastercam. The rest use center of rotation 100% from mastercam.It would be much easier on the operators.

Kinda. G68.2 is what your looking for to match WPC shift in Mazatrol. I use G68 for the integrex because it's parts are always on COR or when I want to use G54.4 to mimick being on COR. I use G68.2 in 5 ax mills because it accounts for deviation from center of rotation like WPC shift in a Mazatrol program. I use G68.4 for angle head work because it's the only one that works with G680 to shift and rotate.

 

If you'll email me a simple 3+2 program I'll post some out for you to compare to yours.

 

PM me for email address.

[JMahon]

I didn't get a chance to get to it today. I'll try in the morning.

 

Just curious, about how far did it set you back for that custom post?

How advanced is this mod?

I've got the post documentation from my reseller and a little post experience...think I could pull it off?

[jlw™]

It may be possible but much of the work is done in the PSB file.

[BNFab]

Lets see the machine, its an e-1600V?? I used to run a few 1550's , bitchin machine! 

[Dave Thomson | Postability]

I don't drop by eMastercam.com often but wanted to simply share that we work to resolve all issues through our standard support mechanism which involves email through your Mastercam reseller.  It looks like this thread has about 3 separate items going on, although all Mazak.  I do recognize some of the names and believe that many of the issues are resolved.  Some were possibly related to default control parameter settings.  If anyone with a Postability post is experiencing any issues, I would highly encourage you to document what you can with supporting samples and send them in to your reseller for our attention.