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:

Must Have HMC Options


g huns
 Share

Recommended Posts

12 hours ago, pullo said:

Just out of curiosity , has Fanuc even bothered  to copy the notion of Basic Rotation like on the Heidenhain ?  I only deal with Heidenhain  and haven't done anything on Fanuc for like 20 yrs...

 

Gracjan

You have lived a sheltered life my friend. :D Like Grievous said there are ways to handle it.

Link to comment
Share on other sites
  • 3 weeks later...

So Fanuc and Enshu have been out since Tuesday to install tilted work plane, G68.2, and tool center point control, G43.4. They asked that we have our post writer come today to make sure everything worked. The guy who writes our post, for a software company NOT named Mastercam, already had a post for a Makino horizontal with those options so he brought it and testing commenced. 

We opted for the 2X4 test.

cpOHiLcl.jpg

I wrote a path that traced along each face of the 2X4 as a 3+1 path using G68.2. And one that did simultainious 4 axis tracing all the way around with G43.4.

Neither worked. At all. 

Enshu has never installed these options, so their guy knows less than me. Fanuc guy is not a 4 or 5 axis expert. Luckily our post guy was able to contact a customer running his post on a Makino and have him take a pic of his parameters that pertain to the G68.2. That at least got the 3+1 program running correctly with G68.2. At that point it was 6pm and told everyone to go home. 

We will have to hash out the G43.4 tomorrow.

If understand TCP correctly, I should be able to MDI a G54 X0 Y1.0, putting my cutter on center and an inch above the 2X4 in Y. Then MDI a G43.4 Z0 H21, putting the tip of tool 21 right on the front face of the 2X4 in Z. Then by placing the machine in jog and rotating the B axis, the tool tip should stay right on the Z0 point as the B axis rotates. The X and Z should move as needed to make this magic happen.

Or am I full of chit?

Link to comment
Share on other sites
1 hour ago, g huns said:

So Fanuc and Enshu have been out since Tuesday to install tilted work plane, G68.2, and tool center point control, G43.4. They asked that we have our post writer come today to make sure everything worked. The guy who writes our post, for a software company NOT named Mastercam, already had a post for a Makino horizontal with those options so he brought it and testing commenced. 

We opted for the 2X4 test.

cpOHiLcl.jpg

I wrote a path that traced along each face of the 2X4 as a 3+1 path using G68.2. And one that did simultainious 4 axis tracing all the way around with G43.4.

Neither worked. At all. 

Enshu has never installed these options, so their guy knows less than me. Fanuc guy is not a 4 or 5 axis expert. Luckily our post guy was able to contact a customer running his post on a Makino and have him take a pic of his parameters that pertain to the G68.2. That at least got the 3+1 program running correctly with G68.2. At that point it was 6pm and told everyone to go home. 

We will have to hash out the G43.4 tomorrow.

If understand TCP correctly, I should be able to MDI a G54 X0 Y1.0, putting my cutter on center and an inch above the 2X4 in Y. Then MDI a G43.4 Z0 H21, putting the tip of tool 21 right on the front face of the 2X4 in Z. Then by placing the machine in jog and rotating the B axis, the tool tip should stay right on the Z0 point as the B axis rotates. The X and Z should move as needed to make this magic happen.

Or am I full of chit?

In jog not sure that will happen. Programmed then yes it should.

Link to comment
Share on other sites
17 minutes ago, C^Millman said:

In jog not sure that will happen. Programmed then yes it should.

Right now, it doesn't do it either way.:rolleyes:

I can't blame the Fanuc guy for not knowing much about things beyond 3 axis. But maybe Fanuc coulda sent us someone who does, instead of just sending the guy who lives closest to our shop.:unsure:

Link to comment
Share on other sites
11 hours ago, g huns said:

Right now, it doesn't do it either way.:rolleyes:

I can't blame the Fanuc guy for not knowing much about things beyond 3 axis. But maybe Fanuc coulda sent us someone who does, instead of just sending the guy who lives closest to our shop.:unsure:

Very few MTB's really know what they're doing. People like James M and few others on this forum that support MTB's are a rare bunch. For Majority of them 3 axis stuff is it. Fanuc sent someone closest to you to save money for them. They still charged you as if it was an out of state technician.

Link to comment
Share on other sites

Anybody got a HMC with a Fanuc 31 with working tilted work plane and tool center point that could check a couple parameters for me?

I believe parameter 19680 should be set to 12, which ours is.

Our 19681 is set to 0. Not really sure what that does. Other than the description that it makes first rotation axis hypothetical when set to 0 and 19696 is a 1, which it is. My rotational axis is NOT hypothetical, it's quite real.:blink:

Our 19682 is set to 1. I'm not sure this is right. This basically says that the rotation axis rotates around the X axis. Shouldn't it be set to 2, so it rotates around the Y axis?

Link to comment
Share on other sites
Just now, huskermcdoogle said:

Are you programming in table coordinates or workpiece coordinates (machine axes) ?  Check status of 19696 bit 5.  I believe you are looking to program in table coordinates.

 

19696 bit 5 is a 0, so yes, table coordinates.

Link to comment
Share on other sites

Just taking a guess, it can't hurt to try it.  Obviously document where you are not before switching a bunch of these.

19681 should be set to 4 likely.  (fourth numbered axis is the rotary)

19682 should be 2.

19686 should be 0

19687 I would set to 0 or 3, but as a hypothetical axis I wouldn't think it would make a difference

19696 bit 0 should be 0

19696 bit 1 should be 1

 

Then make sure you set 19700 and 19702, 19701 should be 0, but as g68.2 is already working, I think you are in good shape there.

Link to comment
Share on other sites
  • 2 weeks later...

After listening to the Fanuc guy tell me, for three straight days, that the post I was supplied with was junk, I finally told him adios. I'll work it out.

Never mind that the post outputs G68.2 and G43.4 according to both Makino's and Matsuura's guidelines.

G68.2 worked fine, but G43.4 did not work correctly if you pre-positioned the B axis. You'd end up with the cutter on the wrong side of the part, cutting in outer space somewhere.

If you did not pre-position the B axis, it worked correctly, but the first move after the G43.4 was EXCITING!

G43.4 G91 Z0. H21
G90
M9
X-1.5374 Y1. Z5.90551 B270. 

X, Y, Z, and B, all at rapid was not ideal.:rolleyes:

Then my post guy called me up and said, you won't believe the call I just got. Another customer with a Makino called and said his machine was behaving the same as mine. The cutter nowhere near the area it should have been cutting after G43.4. They got on the phone with Makino and before they could finish describing the problem, the Makino guy cut them off and told them to go to the machine and set parameter 19754, bit #5 to "1". He said that they occasionally miss it when they set parameters at the factory. They set it, it ran perfectly. So I set it on ours, and it too works perfectly.

So to recap, I paid Fanuc almost $11K to turn on 2 options that they could not make work correctly. Every parameter that was set by their tech was WRONG. I paid my post guy $1200 to provide me with a post and show up for a day. Every parameter that was finally set right came from him.

Link to comment
Share on other sites
1 minute ago, Mark @ PPG said:

even though Fanuc and MTB left you with a huge dissapointment.

It would be nice if there was some good training available on all of the advanced options.  At the very least an informational training course that covers the benefits of each advanced option, and some applications of each.  Fanuc has a laundry list of options available that are very rarely seen, that for highly repetitive parts could potentially slash cycle times by significant margins, and the fact there are probably only a few people in the world that know how to implement them, seems pretty foolish on their part.  The fact that their tech couldn't effectively troubleshoot TCP issues, is down right unaccepatble.  TCP/TWP are not unknown or rarely used functions.  It would seem to me that if they offered some informative courses or material (beyond the useless catalog descriptions), these options would sell themselves.

A one day classroom + one day hands on lab class could easily bring anyone with any basic understanding of what's going on up to speed on the options.  Hell even a simple flow chart for setting the parameters on the three basic kinematic configurations (HH,HT,TT) would likely be all that would be needed to get most techs up to speed to be useful in the field with setting up these functions.

Link to comment
Share on other sites
9 minutes ago, Mark @ PPG said:

NOT surprised at all :)

I'm glad you got it sorted out, even though Fanuc and MTB left you with a huge dissapointment.

I can't blame the MTB. Enshu says these are their first machines to EVER have these options installed. Nobody ever asked for them before. Their customer base is primarily production type work. I guess people are just used to programming from COR and dealing with it.

Based on what I have experienced with Fanuc, I'd guess any MTB commonly using these options has figured it out on their own. 

Link to comment
Share on other sites

Sounds like typical Fanuc. They come out to turn the options on & thats it. They leave it up to the MTB to configure the machines. I have seen the exact some thing with G54.2. They turned the options on on a Mori NH5000 & left. Did not set one parameter. Another time they turned on the the option on a H-Plus 630 & set the parameters incorrectly, so it compensated the opposite direction. Our dealer at the time was clueless as to what the correct parameters were supposed to be. It took trial & error to figure it out.

Link to comment
Share on other sites

Well, I spoke too soon.

They don't run "perfectly". The overall motion is correct, but our locations are off in the X and the Z axis when we do 90 and 270 degree rotations. By about .065" in both.

The part we are cutting has it's X0 set at about .043" off of the machine's X0, which is COR. If that was the number we were off, it would at least make some sense.

Link to comment
Share on other sites

Are you having trouble with G68.2 or G43.4?  I am assuming G43.4.

My suggestion would be to do some testing with the part zero further away from the center so you don't get any sign errors confused.  Start by verifying 19700 and 19702, and verify 19696 bit 5 is a 0, and 19746 bit 4 is 1.   If all of that is correct and you are absolutely sure of that, I'll state the obvious, and ask if things are posting out correctly, and that the mastercam file is setup completely neutral.  I have been dead sure my COR numbers were good in the past but in fact have made math errors, and wasn't, I always, no matter how confident I am in my methods, change use a slightly different method and check again, if they don't agree, figure out why.

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

Are you having trouble with G68.2 or G43.4?  I am assuming G43.4.

My suggestion would be to do some testing with the part zero further away from the center so you don't get any sign errors confused.  Start by verifying 19700 and 19702, and verify 19696 bit 5 is a 0, and 19746 bit 4 is 1.   If all of that is correct and you are absolutely sure of that, I'll state the obvious, and ask if things are posting out correctly, and that the mastercam file is setup completely neutral.  I have been dead sure my COR numbers were good in the past but in fact have made math errors, and wasn't, I always, no matter how confident I am in my methods, change use a slightly different method and check again, if they don't agree, figure out why.

No, G68.2.:(

As to those parameters, 19700 is 0 and 19702 is -1200. The Enshu tech found COR and rezeroed the machine axis to reflect it. I didn't double check him, so I guess he could have screwed up.

And my 19696 bit 5 is a 0 but 19746 bit 4 is a 0 on mine. Is that bad?:blink:

This was a dummy program we were playing with to verify location...

%
O9999
(REGAL ENSHU4X GE590H POST REV 13_06 - APRIL 18, 2018)
( THURSDAY APRIL 19, 2018 - 8:27:30 AM )
G90 G80 G40 G49 G69
G91 G30 Z0.
G90
M906T43
G54
G0 B0. 
X0. Y0. center of part that's 8" wide in X
G43 Z3. H43 z was verified to be 3" from part face
G91 G30 Z0.
G90
G0 B90. 
G68.2 X4. Y0. Z0. I90. J90. K-90.
G53.1
X.5 actual measurement from edge of part was .4353, or +.0647 from where we wish it was
G43 Z6. H43 z was measured to be 5.9327, or -.0673" from where we wish it was
G69
G91 G30 Z0.
G90
G0 B270. 
G68.2 X-4. Y0. Z0. I-90. J90. K90.
G53.1
X-.5 actual measurement from edge of part was .4377, or -.0623 from where we wish it was
G43 Z6. H43 z was measured to be 5.9353, or -.0647" from where we wish it was
G05.1 Q0
G69
G49
M19
G91 G30 Z0.
G90
G91 G30 X0 Y0
G90
M11(UNCLAMP)
G91 G28 G0 B0
G90
M30
%

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...