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:

fanuc G54.2 p1 rotary table dynamic work offset questions


rbu
 Share

Recommended Posts

Hello everyone,

 

I am a mastercam mill level 1 user for several years now and using the search function once in a while but could not find the information i need.

So here are my questions.

 

We have a new vertical machining center with 4 th axis

The machine is a Hartford HCMC-2082 with fanuc 32i with the G54.2 rotary table dynamic fixture offset ( rtdfo ) function.

We are trying to get this function to work but we have no experience with it, and the machine seller doesn't either.

The fanuc book also is not very clear.

 

I have read that ithe function is used a lot on horizontal machines, but can it also be used on a vertical machine with the 4th axis when the parameters are set ?

Does it use G28 which is on a horizontal machine in the center off the table i think, but on a vertical machine the G28 is a fixed position not in the center of the table so is this a problem.

 

What must be set in the G54 page and what must be set in the G54.2 page on the control.

Where do you have to set the workpiece coordinate ( G54 ? ) and where the center off rotation ( G54.2 ? )

 

We have tryed with G10 L21 Pn P and that does fill the x y z and c coordinate from the program in the rtdfo page on the control.

 

May be a example can make things clear.

 

When we know how the function works we want to use it with mastercam in the MPMASTER post, or is this to complicated.

Is there a working fanuc post from mastercam or inhouse or somewhere else.

 

Any help will be very much appreciated.

 

Regards Richard

Link to comment
Share on other sites

I don't know anything about your specific machine, but we use DFO on our Jidic Horizontal. On the Jidic there is a separate page to enter dynamic fixture positions. Similar location to where you would enter you standard fixture offsets. That's assuming you have the option turned on in the machine.

 

We have one machine that uses DFO, and MasterCam works without doing anything special. You may need to add the codes to activate and deactivate it. We have another machine that uses TCPC, and we had to have help getting MasterCam to work with that style of programming. Collin helped us out with that.

 

I'm not familiar with G10 L21, we do use G10 L2, and G10 L20 for setting work piece origin offsets and additional work piece offsets. A quick search for G10 L21 didn't turn up anything in my Fanuc book. So I can't help you with that.

Link to comment
Share on other sites

thanks for your reply,

 

We have the separate page where we can enter 8 dfo,s.

Do we have to set the workpiece x,y,z, and c position in there and not use G54 at all.

 

On a horizontal you have a fixed center of rotation where the G54.2 calculates from which was allready set on your machine, but on a vertical we have to set that somewhere in the control and depends on the position of the rotary table.

That can be the reason why it is not working in our case yet.

 

Do you have an example program with a few different planes.

 

How do you set the parameters for different views in mastercam to put out G54.2 instead of G54, G55, G56 etc.

Link to comment
Share on other sites

I am running a Makino A51nx with the 31i control and I assume the operation guidelines are pretty similar. If so you will need to set two offsets to run DFO and they aren't all that intuitive. The first is G54 and the second is G54.2. The G54.2 offset corresponds to your rotary table axis position in Y and Z and the G54 corresponds to the distance from that axis to your part offset. You machine manufacturer should have the information on exactly how you set it up but I am 99% sure that your part Y and Z positions (G54 Y and Z values) are the distance from the rotary axis position in Y and Z, assuming the rotary axis is parallel to the machine's X-axis.

 

If your machine runs the same as mine you will need to post G54 then G54.2P1. G55 would be G55 then G54.2P2. G54.2P0 cancels DFO. There might be a switch in your post to enable posting DFO.

  • Like 1
Link to comment
Share on other sites

In our case the Fixture offset is used to indicate the centerline of the rotary, and the Dynamic offset is used to indicate where the origin is on the part from the centerline of the rotary.

 

In our MasterCam file, we do nothing special. We don't use multiple fixture offsets. all of our program use G54, regardless of how different planes there are.

 

We only use dynamic when doing full 5th axis type of cuts. For 3+2, we use a rotation macro. In your case you could use multiple work offsets. But when you are doing Multi-axis type of cuts, use top view, and the dynamic will take care of positioning. I don't really see a need for ever using multiple dynamic offsets, but I'm sure someone here has a situation where that might be needed.

 

I hope this makes sense.

 

Here is a sample of a simple start up of the DFO

 

T1(FTN 21200040 - 2 finish face mill)
M6
G0 G54 G90 X-2.3327 Y1.8645
B-90. A84.
S6500 M3
M10
M12
G43 H1 Z8.
G0 G54.3 P1 G90
X-2.3327 Y1.8645
B-90. A84.
M8
Z1.6

Link to comment
Share on other sites

thanks bob

The control is also a 31i not 32i so it should be the same except that it must be set up for a vertical.

What you are saying looks like the book is telling and what we have tried,

We will try again with your info.

We have to inform at the manufacturer how to set the parameters.

 

Do you have an example program, and how did you set up your post.

Link to comment
Share on other sites

%
O0000(TOMBSTONE_FACING)
(WCS POSITION)
#580=0 (PART X POSITION)
#581=0 (PART Y POSITION)
#582=-29.13385 (PART Z POSITION)
#583=0 (PART B POSITION)
G53
G90 G10 L2 P1 X0. Y#581 Z[-29.13385] B#583
G90 G10 L21 P1 X[#580] Y0.0 Z[#582+29.13385] B0.0
#3006=0 (UNPROVEN PROGRAM)
#575=0 (PROGRAM PALLET ASSIGNMENT)

 

This is my post header. It is set up so an operator can probe the part and enter the values into macro variables #580-#583. I also have my 5-axis post set up the same way. Just type in the offset position and the machine does the rest.

 

Also, keep in mind this is set up for my horizontal machine and I know exactly where the B-axis is so those values are hard coded (-29.13385, etc...)

Link to comment
Share on other sites
We have a new ... with fanuc 32i with the G54.2 rotary table dynamic fixture offset ( rtdfo ) function. We are trying to get this function to work but we have no experience with it, and the machine seller doesn't either.

If I had a dollar every time I heard about a Machine Tool Dealer/Seller that has no clue about how higher-end functions work, I'd be doing alright.

 

 

The fanuc book also is not very clear.

If I had a nickel for every time the FANUC book wasn't clear on something I'd be on the Forbes list.

 

Let's take a time-out for a second...

 

I have a question;Richard, do you know for certain that the RTDFO option has been properly configured on/for your machine? That HAS to be done first or you're in for nothing but grief and heartache.

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...