Jump to content

Welcome to eMastercam.com
Register now to gain access to all of our features. Once registered and logged in, you will be able to create topics, post replies to existing threads, give reputation to your fellow members, get your own private messenger, post status updates, manage your profile and so much more. This message will be removed once you have signed in.
Login to Account Create an Account
Photo

Dynamic tool compensation

- - - - -

  • Please log in to reply
16 replies to this topic

#1
Shawn'ald

Shawn'ald

    Member

  • Members
  • PipPip
  • 280 posts
We are looking at getting into 5ax machining, and are looking at machines (Matsura,Mori). I have herd not to get one that doesn’t have dynamic tool comp. I did a search for this but I am still confused as to what this means. I thought initially it had to do with MC or your cam software. If you guys could give me some insight to what this is that would be very helpful.

Thanks, Shawn...

#2
Crazy^Millman

Crazy^Millman

    Regular Guy

  • Members
  • PipPipPip
  • 12,020 posts
  • Location:Murrieta Ca
Best way I can explain it is the ability to program all of your tools in a Cam program to a certain length. The the machine will automatically compensate for the difference in the actually length when doing 5 axis cuts. The reason this is important is that if a tool changes length by .005 every time it is set-up and you do not have this on that machine you have to repost the code. Now if some person has put 1 or 2 hours on the floor tweaking that program, it is all lost. Also if you need to lengthen or shorten a tool at the machine it does not have to be re-posted. Most machines that have this use a tooleye which also means it is quicker to set-up the machine and get jobs running faster.

I would tell anyone looking to buy a 5 axis and spend that amount of money and then get cheap on this option needs to just not bother buying the machine you are not ready and really do not want to get into 5 axis machining.

HTH

#3
Bruce Caulley

Bruce Caulley

    Advanced Member

  • Members
  • PipPipPip
  • 4,067 posts
  • Location:Brisbane, Australia
Basically it means that the control monitors the position of your datum relative to its centre of rotation for each axis and compensates the motion to suit. Without it you would be required to have your model origin in MC as the centre of rotation. With it you can put your datum anywhere you want.

One example would be machining a helix on a cylinder. In a standard machine you would need to make sure that the cylinder was concentric with the rotary axis. If you have dynamic comp, it doesn't matter if the cylinder is offset as the machine will use the other axes to compensate as it rotates.

Dynamic comp allows you to put mount the part anywhere on the table without worrying where the datum was in the CAM file.

Bruce

#4
Bruce Caulley

Bruce Caulley

    Advanced Member

  • Members
  • PipPipPip
  • 4,067 posts
  • Location:Brisbane, Australia
Ah, I was talking about something slightly different. In a head-head machine Crazy's example is correct. In my case I was refering to a table-table machine.

Bruce

#5
Shawn'ald

Shawn'ald

    Member

  • Members
  • PipPip
  • 280 posts
Ok cool! So it doesn’t have to do with the cam software. Thanks guys, that makes more sense. The only other question that I have would be do all machines offer this as an add on or do only certain controls deal with this? Thanks again..

#6
Bruce Caulley

Bruce Caulley

    Advanced Member

  • Members
  • PipPipPip
  • 4,067 posts
  • Location:Brisbane, Australia
It is an option an pretty much all fanuc based machines. Definately ask about it when talking to a machine supplier. I know that Haas do not offer this.

Bruce

#7
Steve Biehl - Cimquest Inc

Steve Biehl - Cimquest Inc

    Advanced Member

  • Resellers
  • PipPipPip
  • 1,514 posts
pretty much standard on newer Heidenhain and Siemens controls. But still ask.

+1 on Crazy, don't bother without it.

#8
Shawn'ald

Shawn'ald

    Member

  • Members
  • PipPip
  • 280 posts
Thanks alot guys. I figure the Mori or Matsuura should have it as an option then..

#9
MMT-USA

MMT-USA

    Member

  • Members
  • PipPip
  • 71 posts
Shawnald, I popped you an email if you need some information I'd be glad to help.

#10
hsm400

hsm400

    Member

  • Members
  • PipPip
  • 33 posts
Moris have it....Matsuuras don't. They band-aid it with CAMPLETE, which is a hassle, in my opinion.

FYI...the Fanuc based controls need to have the rotarys at zero to activate it, while Heidenhain and Siemens controls can activate it anywhere.

It is relativly a new feature for Fanuc, but Siemens and Heidenhain have been doing it for a while.

#11
Mic

Mic

    Member

  • Members
  • PipPip
  • 282 posts
  • Location:Denmark
hsm400-> Not true.

Matsuura has both G43.4/G43.5 ( RTCP ) G68.2 ( Tilted work plane ) and G54.4 ( work setup error compensation ) as an option for all their 5X machines. It comes as 5X related option package.

And the newest release of the Fanuc 30-i don't need rotrarys at zero to activate. But this is only about 6 month old.

For a Matsuura you should go for the Matsuura control option called 19.3. This is a combination of all the Fanuc hignspeed stuff, dataserver and the 5X package.

#12
hsm400

hsm400

    Member

  • Members
  • PipPip
  • 33 posts
Mic, in the US, Methods Machine Tools doesn't seem to push these features for whatever reason.

I knew Fanuc was working on this issue, but I have yet to see any Fanuc control that didn't behave like this. Maybe I'm working with old data, thanks for the correction!

#13
Post dept

Post dept

    Member

  • In-House Solutions
  • PipPip
  • 273 posts
Huh, I haven't seen a fanuc that can start at an angle other than 0 with G43.4. That will be sweet!

You're right, totally has nothing to do with your CAM software.....but a lot to do with the post.

Sounds like you're looking at a trunnion. Definitely get the G54.2. It works for both 3+2 and 5-axis. G43.4 isn't really doing much more for you except the ability to use diameter wear comp for swarf machining (G41.2).

BTW, Matsuuras do have the G54.2. Not sure about G43.4 though. Mori has both.

Good luck with it Shawnald!

Brett

#14
Mic

Mic

    Member

  • Members
  • PipPip
  • 282 posts
  • Location:Denmark
For 5X toolpaths G43.4 is the way to go. That way you don't have to think about inversed time feedrate. And G54.2 don't compensate for the small shift between A ( B on some machines ) and C axis. Even the most accurate machines has a small shift here, normally within 30 microns, but this could still cause some problems if this isn't being compensated. I would always recommend G43.4 for 5X and G68.2 for 3+2 as both these functions does take care of the small shift between the axis's.

If the Matsuura has G54.2 it usually also has G43.4 as both these are bundled in the 5X Matsuura software package. But I think Matsuura now are using G54.4 instead of G54.2

#15
Shawn'ald

Shawn'ald

    Member

  • Members
  • PipPip
  • 280 posts
Thanks guys for the replies, and MMT-USA I sent you an email so you can tell what Matsuura offers!! graemlins/cheers.gif

#16
MMT-USA

MMT-USA

    Member

  • Members
  • PipPip
  • 71 posts
Mic ,

You are correct. G54.2 doesn't compensate for the "Stacking error" so to speak. The new function G54.4 has now replaced this function.

You are also correct on the "Dynamic" functions for Fanuc controls.

TCPC = 5-axis transformation
TWP = 3+2-axis transformation

We program these functions with G-code relative to the part "WCS" rather than the "MCS".

hsm400,

We sell our 5-axis Matsuura's with a set package. This includes 5-axis transformation functions and CAMplete TruePath software for both platforms.

It's one thing to have the functionality, and it's another thing to get good g-code to support it.

#17
JMC

JMC

    Advanced Member

  • Members
  • PipPipPip
  • 928 posts
  • Location:All of North America

quote:


Moris have it....Matsuuras don't. They band-aid it with CAMPLETE, which is a hassle, in my opinion.

Producing the actual code is a band-aid???