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:

5 Axis program help needed


PAnderson
 Share

Recommended Posts

I really need some help here trouble shooting a Fanuc program and possibly a post. I am not a day to day, all day, user of Mastercam. Only in support of our showroom here at Doosan. I started 5 axis here on a Heidenhain control. Machine and post were flawless. Now, I have to get this program working on a Fanuc 31i/B5.

First, my post was only having the machine move over the part but as the A and C axis rotated, the tool was not following the part as it rotated. I spoke to a colleague at a dealership who said his programs also have G68.2 to get the tool out over the top of the part as it rotated. My post does not post this out and he sent me a sample. But it still does not work but I think there is probably a different reason and I have no clue. Please see the below sample. The middle of the program was deleted as not needed to show the problem. I am programming from the top of the part being Z0., using Top-Top-Top.  Any help would be greatly appreciated. I am trying to get this going for one of our dealers open houses.

Thanks,

Paul

%
O0200(T1 ROUGH BLADES)
(MASTERCAM - X11)
(DATE      - 2017.09.19)
(TIME      - 9:21 AM)
(T1-6MM TAPERED ENDMILL-H1-D1-D0.2362"-R0.1181")
G00G17G20G40G80G90
G91G28Z0.
G90A0.C0.
N1
(BLADE ROUGH)
T1M06(6MM TAPERED ENDMILL)
G54G17G90
G00A-73.856C103.189
G68.2X-2.7717Y-.7499Z-.3781I-256.811J73.856K180.0
G53.1
X0.Y0.
G43H1Z1.S11750M03
G49
G69
G90G43.4H1
X-2.7717Y-.7499Z-.3781  (Everything seems to work until this line until G43.4 is read, then the machine  goes almost to home position minus tool length offset

where the absolute Z reads Z-.3781. I have no idea what is going on here and not even sure if this program structure is correct.)
G94
G05.1Q1R10
X-2.5161Y-.69Z-.4541
G01X-2.142Y-.6024Z-.5653F60.
X-2.1428Y-.5741Z-.5382A-73.875C103.181F141.
X-2.1453Y-.5036Z-.4744A-73.904C103.142
X-2.1466Y-.4326Z-.4094A-73.942C103.106
X-2.1459Y-.4275Z-.4046A-75.071C103.597
X-2.1435Y-.4232Z-.4005A-76.117C104.048
X-2.1395Y-.4195Z-.3969A-77.165C104.494
X-2.1339Y-.4166Z-.3939A-78.298C104.972
X-2.1282Y-.415Z-.3922A-79.605C105.519
X-2.1242Y-.4154Z-.3924A-80.482C105.882
X-2.1217Y-.4179Z-.3946A-81.357C106.244
X-2.1208Y-.4223Z-.3987A-82.666C106.78
X-2.12Y-.4895Z-.4619A-82.604C106.857

 


G00X-.0449Y-1.1377Z-.3006
X-.0347Y-2.4618Z.0419
G49
G05.1Q0
M05
M09
G91G28Z0.
G28X0.Y0.
G90A0.C0.
M30
%

 

Below is the way my post codes this program. This ignored the rotations altogether. Totally no clue what is going on here. I guess I was spoiled on the Heidenhain.

O0100 (T1 ROUGH BLADES)
(MASTERCAM - X11)
(DATE      - 2017.09.19)
(TIME      - 9:21 AM)
(T1   - 6MM TAPERED ENDMILL  - H1   - D1   - D0.2362" - R0.1181")
G00 G17 G20 G40 G80 G90
G91 G28 Z0.
G28 X0. Y0.
G90 A0. C0.
N1
 (BLADE ROUGH)
T1 M06 (6MM TAPERED ENDMILL)
G54 G17 G90
G00 A-73.856 C103.189
G43.4 H1 X-2.7717 Y-.7499 Z-.3781 S11750 M03
G94
G05.1Q1R10
X-2.5161 Y-.69 Z-.4541
G01 X-2.142 Y-.6024 Z-.5653 F60.
X-2.1428 Y-.5741 Z-.5382 A-73.875 C103.181 F141.

Link to comment
Share on other sites

Well G43.4 is TCP, and by the sounds, this is only part of what your trouble is.  How is TCP setup in the machine?  Are the Kinematic offsets for TCP setup in the control?  Is the post setup to post in table or workpeice coordinates, and does that match what the machine parameter setting?  This stuff isn't trivial for someone that hasn't set this stuff up before, but it isn't rocket science either.  Being that it sounds like you are with the MTB, I would imagine you should have the support to get the machine side of things figured out with ease.  Figure out the details of what the machine is looking for to use TCP and TWP and you will have a good foundation to get the support you need to get the post worked out.

What post are you using?

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

Well G43.4 is TCP, and by the sounds, this is only part of what your trouble is.  How is TCP setup in the machine?  Are the Kinematic offsets for TCP setup in the control?  Is the post setup to post in table or workpeice coordinates, and does that match what the machine parameter setting?  This stuff isn't trivial for someone that hasn't set this stuff up before, but it isn't rocket science either.  Being that it sounds like you are with the MTB, I would imagine you should have the support to get the machine side of things figured out with ease.  Figure out the details of what the machine is looking for to use TCP and TWP and you will have a good foundation to get the support you need to get the post worked out.

What post are you using?

Thanks Husker, I thought TCP would be all I needed but I guess I am wrong. Support from the factory, unfortunately, will be non-existent. Generally, these machines come in OK.

I use a post from Postability. Their Heidenhain post worked right out of the box, flawlessly. But I find Heidenhain to be way more ahead of Fanuc as to control setup. Are you aware whether a G68.2 should be used in conjunction with G43.4? I tried changing Par. #19696 bit 5 to a 1 and a zero and get the same results. I also compared this machines parameters to a known machine from the recent past and all the 5 axis parameters were identical except for the kinematics parameters, 19700 thru 19707, I think. Did you happen to see anything out of the ordinary with the code sections I posted?

 

Regards,

Paul

  • Like 1
Link to comment
Share on other sites
14 minutes ago, PAnderson said:

Support from the factory, unfortunately, will be non-existent.

As it sounds like you are working with a dealer.  How do customers get decent support if a dealer can't?

-------

The only thing after a quick look in the first sample that doesn't seem ordinary to me would be that fact that G68.2 is being called then canceled (G69) before any work is done.  With the second sample, the machine rotates, activates G43.4, and then continues, this I would say is typical for full 5 or continiuous rotary motion.  G68.2 is typically for a temporary shift for toolplane type work, or shifting the zero point from the rotary center (where you work offset should be) to another point, or vise versa.

I'll be the first person to tell you that I don't have any experience with TCP on a table table type machine.  Only H/H and H/T configurations with a Fanuc Control.  It's all related, and is the same general theory, but totally different at the same time, as there are many options, which it seems you are at least decently familiar with already.

Otherwise without a sample file its hard to tell.

  • Thanks 1
Link to comment
Share on other sites

I'm pretty sure there are machine parameters that are not properly set

There are parameters in the control that tell  the control the distance from the spindles gage line to the  center of rotation

of the rotary axis.

It uses these values, along with the tool length offset to do all the math needed to drive the tip of the tool.

I'd be willing to bet those parameters are set to zero.

 

Link to comment
Share on other sites

A quick experiment

This will only work on head/head machines

IF .. you know the pivot distance of the machine

add that value to the tool length offset and run the file

If it looks right,.. or even only looks better, the parameters I mentioned in my previous post are not properly set

 

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

As it sounds like you are working with a dealer.  How do customers get decent support if a dealer can't?

-------

The only thing after a quick look in the first sample that doesn't seem ordinary to me would be that fact that G68.2 is being called then canceled (G69) before any work is done.  With the second sample, the machine rotates, activates G43.4, and then continues, this I would say is typical for full 5 or continiuous rotary motion.  G68.2 is typically for a temporary shift for toolplane type work, or shifting the zero point from the rotary center (where you work offset should be) to another point, or vise versa.

I'll be the first person to tell you that I don't have any experience with TCP on a table table type machine.  Only H/H and H/T configurations with a Fanuc Control.  It's all related, and is the same general theory, but totally different at the same time, as there are many options, which it seems you are at least decently familiar with already.

Otherwise without a sample file its hard to tell.

Husker, there is no direct factory presence here in the US other than service techs here. And with the time difference and language barrier, we can't expect much help from Korea. Nor do I want to, we need to do this ourselves. As for the dealer I am working with?, pretty good but don't have any 5 axis guys. Don't get me started.

I never thought TCP should be used together with TWP, 2 separate tools in my opinion but another dealer tech uses that method with success apparently. Could be parameters but nothing seems out of place and this program did run with no problems on a TNC640. But, it's either the post or the parameters and I am on my own here.

 

Thanks for the input, I appreciate everything.

 

Paul

Link to comment
Share on other sites
30 minutes ago, gcode said:

A quick experiment

This will only work on head/head machines

IF .. you know the pivot distance of the machine

add that value to the tool length offset and run the file

If it looks right,.. or even only looks better, the parameters I mentioned in my previous post are not properly set

 

gcode,

These parameters, 19700-19705 are populated, and with good numbers. But they are measured from home position. So my G54 is set to X-200.0MM, Y-319.981MM and my Z is set to the difference between the Z-550.12 and the height of fixture/part, since this is programmed from the top of the part.

 

Thanks for your input also,

Paul

N19700Q1L1P-200.0L2P0.0
N19701Q1L1P-319.981L2P0.0
N19702Q1L1P-550.12L2P0.0
N19703Q1L1P-0.002L2P0.0
N19704Q1L1P-0.017L2P0.0
N19705Q1L1P0.12L2P0.0

 

 

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

A quick test to verify that would be to put the first position after the  g43.4 on the g43.4 line.  That would tell you real quick if that is the issue or not.

Thanks guys, per my second example in the first post, that is how my post spits out code, if I read this correctly.

T1 M06 (6MM TAPERED ENDMILL)
G54 G17 G90
G00 A-73.856 C103.189
G43.4 H1 X-2.7717 Y-.7499 Z-.3781 S11750 M03

 

Paul

Link to comment
Share on other sites
2 hours ago, PAnderson said:

I never thought TCP should be used together with TWP

Well based on the code he isn't...  He's canceling the TWP before activating the TCP.  Which IIRC TWP cannot be activated before TCP and vise versa.  Looking at the yellow bible g43 is allowed in g68.2, but not specifically g43.4, and g69 needs to be modal to call g43.4.

 

Link to comment
Share on other sites

The first example at the beginning was given to me as a sample program from another tech that swears that works for him. Never heard of that but I admit I am learning. I would rather not use the G68.2. It does seem odd, 2 different uses and purposes. I have used G68.2 extensively in the past.

It seems to me that even though the control takes G43.4 and TCP flashes on the screen, it is actually not working because it will not track the rotating part. What is this "activate/deactivate" G43.4 disable motion parameter you speak of. And why would you need that?

 

Paul

Link to comment
Share on other sites
3 minutes ago, PAnderson said:

Thanks guys, per my second example in the first post, that is how my post spits out code, if I read this correctly.

I missed that when commenting about what JLW put up.  Yeah, seems to me something else is funky other than that.

 

2 hours ago, PAnderson said:

N19700Q1L1P-200.0L2P0.0
N19701Q1L1P-319.981L2P0.0
N19702Q1L1P-550.12L2P0.0
N19703Q1L1P-0.002L2P0.0
N19704Q1L1P-0.017L2P0.0
N19705Q1L1P0.12L2P0.0

Based on these is the rotary platten close to being on the c/l of the A axis (.12mm below)? 

Also check 19746 bit 4.

 

Link to comment
Share on other sites

If you fire G43.4 and motion on activation is set to on it will try to move the linear axes to keep the tool tip in the same place.

If it is off, it will rotate the machine without moving the linear axes.  Same as plain old G43 with or without motion.  I always set mine to no motion on activation and cancel as it can cause some booboos if you're not careful.

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

I missed that when commenting about what JLW put up.  Yeah, seems to me something else is funky other than that.

 

Based on these is the rotary platten close to being on the c/l of the A axis (.12mm below)? 

Also check 19746 bit 4.

 

19746 bit 4 is 0 but I am not using 3D cutter comp. And yes, the table surface is technically the center of rotation, but .12MM below.

Edited by PAnderson
left something out
Link to comment
Share on other sites
22 hours ago, huskermcdoogle said:

Set #19696 bit 5 to a 0 and 19746 bit 4 to 1.  That will put it in table coordinate system.  Previously with 19746 bit 4 set to 0, changing 19696 bit 5 won't do anything, it will remain in workpeice coordinate system.  I would just try this and see if the behavior changes to something favorable.

Husker,

You da' man. That was it. #19746 is somewhat outside the beginning of 5 axis parameters, at least in the parameter book. Didn't think to look there.

Thanks so much,

Paul

P.S. Thanks to everyone else that piped in too.

Link to comment
Share on other sites

Ask and ye shall receive. This is a setup part. It was run originally on our VC630 with Heidenhain TNC640. This one is in our DNM350 with Fanuc 31i/B5 control. Testing the post and machine settings.

Thanks for the help. Who would have thought there was a parameter that determines whether another parameter is used or not?

 

Paul

DNM350_Impellor.mp4

  • Like 7
Link to comment
Share on other sites
On 9/28/2017 at 5:30 AM, PAnderson said:

Ask and ye shall receive. This is a setup part. It was run originally on our VC630 with Heidenhain TNC640. This one is in our DNM350 with Fanuc 31i/B5 control. Testing the post and machine settings.

Thanks for the help. Who would have thought there was a parameter that determines whether another parameter is used or not?

 

Paul

DNM350_Impellor.mp4

jealous!:unworthy:

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...