Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Genos M460V-5AX help needed.


danielm
 Share

Recommended Posts

I cant explain why my tool path is looking like it is.  This is my first trunion style 5ax.  Its a simple 5ax curve path on an arc segment surface.  I'm starting to think that there is a parameter in the machine thats causing the toolpath to be out.  X 'looks' good.  Y is off negative by maybe .500"  and the tool tip does not follow the curvature of the surface consistently ie its deep and shallow by as much as .050" .  Centerline of A is per factory.  C zero checks out.  My machine def looks correct and I get same result with different posts that are supposed to be proven for this machine.

Can anyone comment on critical 5-ax parameters on this control OSP-P300MA-H that I should look out for....bit settings etc?   

Thanks in advance.

DM

 

Link to comment
Share on other sites

Work Coordinate shift process where you touch off the part like a 3 Axis and the machine then takes all the 5 Axis movement that was programmed from that Zero and then adjust the code to run in that new position without it having to be the exact position like it would have to be if you programmed from Center of rotation. The idea is to let the machine do all the heavy thinking so to speak and solve difference in part position to where it really is on the machine.

  • Like 1
Link to comment
Share on other sites
6 minutes ago, danielm said:

G169 appears to be the equivalent to DFO for this machine.

 

Manual says:  G169      Tool length offset at cutting edge ON 

 

Doesnt make sense to me....but I turned it off and damn near crashed.

DFO in an Okuma is G605. Not the same thing as TCPC (G169). G605 is used for 3+2 positioning. G169 is used for full five axis cutting. Did you run the 5 axis auto-tune to make sure the rotation centers are set correctly?

Link to comment
Share on other sites
5 minutes ago, danielm said:

no.  Please school me on 5 axis auto tune.   I'm looking in the manuals now.....

PM me your email address and I will email you the MU series 5 axis training manual. It gives a more simplified explanation of the auto tuning use than the full manual.

Link to comment
Share on other sites
10 hours ago, Mick said:

G605 is DFO? We use CALL OO88 but then, they probably updated since then.

Essentially DFO does the same thing as CALL OO88 but with some differences. As Greg said, CALL OO88 only updates the XYZ offset position so you still need to post the rotary moves. DFO is modal and dynamic. Once G605 is active any rotary move will automatically update the XYZ offset position. The one limitation is that you have to post rotary moves by themselves, no linear on the same line. The biggest advantage and need for developing the DFO was being able to use it in conjunction with slope machining. If you have a casting or other organic part that you need to align the coordinate system to using slope, you can also turn on DFO to maintain that alignment for other rotary positions. 

  • Like 2
Link to comment
Share on other sites
8 hours ago, YoDoug® said:

Essentially DFO does the same thing as CALL OO88 but with some differences. As Greg said, CALL OO88 only updates the XYZ offset position so you still need to post the rotary moves. DFO is modal and dynamic. Once G605 is active any rotary move will automatically update the XYZ offset position. The one limitation is that you have to post rotary moves by themselves, no linear on the same line. The biggest advantage and need for developing the DFO was being able to use it in conjunction with slope machining. If you have a casting or other organic part that you need to align the coordinate system to using slope, you can also turn on DFO to maintain that alignment for other rotary positions. 

Thanks for the comprehensive explanation Doug. When was G605 made available?

Link to comment
Share on other sites
18 minutes ago, Mick said:

Thanks for the comprehensive explanation Doug. When was G605 made available?

It is a new option that has not been around very long. I just learned of it late last year. I do not know how long they were working on it. 

  • Like 1
Link to comment
Share on other sites
  • 1 year later...

Straight from the horse's mouth: 

The conventional fixture offset command (CALL OO88) had to be specified each time the angle of the rotary axis is changed. Dynamic fixture offset function(G605), however, detects the angle change with the rotary axis during function mode ON automatically, executing the process equivalent of the conventional fixture offset command. As a result, the user does not have to execute the fixture offset command upon each time the angle of the rotary axis is changed. -5-AXIS MACHINING FUNCTION MANUAL Section 13 

It is OSP-P300 specific.  

That error likely means that you don't have everything in the G605 line you need. However, what you are looking to do would be more of a G169 thing. TCPC (G169) is intended to be used for things like 5 axis contouring and 5 axis surfacing. CALL OO88 is used more for positioning to a plane in a 3+2 fashion. (Though I use it before I enable my G169 to preposition my tool to the clearance plane) G605 is for drilling holes around an eccentric shaft. To be honest, it's a lot of work to set up on the code end and CALL OO88 does the same thing EXCEPT you have to kill your drilling cycle, run a new CALL OO88 line, rotate to the new position, then reactivate your drilling cycle on every hole that is at a different rotation. It would be a lot to write by hand, but then again, if you are hand programming a 5 Axis, slap the hand, commend your self for the outstanding achievement, then get a CAM software.

As for autotuning, I attached a file that I made a few months ago that gives a crash course on a bunch of P300 mill features. Though, because I am lazy and because I don't like G605, it isn't mentioned in there. 

OSP-300MA QUICK GUIDE.pdf

Link to comment
Share on other sites
  • 1 year later...
On 6/20/2018 at 12:08 AM, Greg Williams said:

CALL OO88 does not update the rotary axis positions only the XYZ is updated with this MACRO

Ive just recently dicovered this ( 5 axis newbe with a very cool machine) is there a way to update rotary axis? 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...