Cutter compensation 1

[sitti]

Hello Everybody,

I want to use cutter compensation on a machining center with Fanuc, but I don't know what is wrong. I have a post processor, wich generates the G41, and G42 commands, but the machine is not doing it. It works like if it were programmed with G40. If I put in any radius wear, it doesn't matter.
The machining with manual programming is this (this is working well):
.
.
.
G0G43Z5.H5
G0Z1.95
G1Z-7.5F200.
G1G41Y52.8F70
G3X0.Y44.8R8.
G2X19.23Y41.63R60.
G2X33.5Y21.74R20.998
G1Y12.
G2X21.5Y0.R12.
G1X11.17
G2X9.63Y.72R2.F40
G3X-9.63Y.72R12.5
G2X-11.17Y0.R2.002
G1X-21.5F70
G2X-33.5Y12.R12.
G1Y21.74
G2X-19.23Y41.63R21.
G2X0.Y44.8R59.995
G3X8.Y52.8R8.
G1G40Y57.8
G1Z300.F2000
.
.
.

And a similar one with NX:
G00 X-14.343 Y-7.43 Z3.3 S800 M03
Z-5.2
G01 Z-8.2 F110.
G41 X-14.93 Y-5.
G03 X-19.512 Y-2. I-4.582 J-2.
G01 X-27.5
G02 X-46.5 Y17. I0.0 J19.
G01 Y26.16
G02 X-31.597 Y51.503 I29. J0.0
X31.597 Y51.503 I31.597 J-56.803
X46.5 Y26.16 I-14.097 J-25.343
G01 Y17.
G02 X27.5 Y-2. I-19. J0.0
G01 X11.524
G02 X5.961 Y.752 I0.0 J7.
G03 X-5.961 Y.752 I-5.961 J-4.552
G02 X-11.524 Y-2. I-5.563 J4.248
G01 X-19.512
G03 X-24.095 Y-5. I0.0 J-5.
G40
G01 X-24.682 Y-7.43


The only difference I find is that CAM program is generated with "I" and "J". Can it be the problem? If yes, how can I change it to "R"?
Or what else can be false?
In Planar Profile I turn on cutter compensation in Non Cutting Moves -> More -> Cutter Compensation. If it's correct.

I tried to check the post processor in Post Builder, but I couldn't find the pui file, only the def and tcl files. Maybe because it's an old postprocessor, which was made for NX3?

Thank you for any help and informations.

 

[looslib]

Check the Fanuc manual, it may be that you need an explicit G01 on the line with G41, G40 & G42 codes.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[DaSalo]

I don't see any tool call or offset word (H) in your last example. Your control won't pick up your offset unless you tell it to read the parameter. Every time you change the offset you need to tell the control to read the new entry. In your first example you have G43 followed by an 'H" word in your first line which tells the control to read the tool length offset. The control probably reads the wear offset at the same time (not 100% sure of this, some controls read the offset table at the tool call). This is how you are picking up this information and making it available for the G41 and G42 commands to apply. In your last example you never tell the control to read the offset table so the G41 and G42 do nothing. In your last example you are turning off cutter comp while in circular interpolation mode (G3). Some controls don't like that but I don't think that should normally be a problem for a Fanuc control. Siemen's Arcramatic controls require you to be in linear mode before programming G40, for example.

 

[shags72]

We need to really see you're whole code from both. At least the first operation to see all the codes involved. It might need a D code if the offsets aren't in the tool call like T0101 or the like. It is being turned on on a linear move though it doesn't have the G01 in front as it is modal but that shouldn't be it. I think that it doesn't know which offset register it is using.

 

[sitti]

I checked the manual, and tested the machine with G41. If I write a simple program manually,
with cutter compensation, everything works fine. The program is the following:

G40 G17 G94 G80 G90 G21
M6 T20 (DIA. 10 END MILL)
G43 G00 G54 X20 Y20 Z10 S800 H20 M03
G41 D20 G01 X0 Y0 F100
Y-20
X-20
Y0
X5
G40
M30

This is just to be sure, how the cutter compensation works.

Some geometrys of the part I want to machine needs the possibility of tool wear compensation.
One of it is the following:

N2 T20 M06 (DIA. 10 END MILL)
G43 G00 G90 G54 X16.524 Y-11. Z5.8 S800 H20 M03
Z-4.2
G01 Z-7.2 F110.
G03 X11.524 Y-6. I-5. J0.0
G02 X4.371 Y-2.462 I0.0 J9.
G03 X-4.371 Y-2.462 I-4.371 J-3.338
G02 X-11.524 Y-6. I-7.153 J5.462
G03 X-16.524 Y-11. I0.0 J-5.
G01 Z-4.2
G00 Z5.8
G00 X-14.93 Y-7. Z3.3 S800 M03
Z-4.2
G01 Z-7.2 F110.
G03 X-19.512 Y-4. I-4.582 J-2.
G01 X-27.5
G02 X-46.5 Y15. I0.0 J19.
G01 Y24.16
G02 X-31.597 Y49.503 I29. J0.0
X31.597 Y49.503 I31.597 J-56.803
X46.5 Y24.16 I-14.097 J-25.343
G01 Y15.
G02 X27.5 Y-4. I-19. J0.0
G01 X11.524
G02 X5.961 Y-1.248 I0.0 J7.
G03 X-5.961 Y-1.248 I-5.961 J-4.552
G02 X-11.524 Y-4. I-5.563 J4.248
G01 X-19.512
G03 X-24.095 Y-7. I0.0 J-5.
G01 Z-4.2
G00 Z3.3
G91 G28 Z0.0

This program is generated with NX, without any cutter compensation settings in planar profile.
So this is what I want to post with cutter compensation.

I think the cutter compensation is not available in our post processor. How can I check it? If it is, how can I turn it ON in the operations, for example in planar profile?
If I am right, and it is not set, can I modify it with Post Builder?
And the last thing is, the 'I' and 'J'. Can I change it to 'R' in post processor too?

 

[looslib]

If your company wriote the posts, then it is all changeable.
Postbuilder is very flexible in what it can do, but does take some work in learning how to create efficent posts.
From your first sample, you do seem to have cutcom enabled as the NX sample has the g41/g40 code in your listing.
You may need to look at the tool change command and see that it is putting out the H code for that tool when the tool is loaded.

As to how exactly to do it, I haven't used Postbuilder since NX1, so someone with more recent experience will have to answer. From what I rememeber, launch PB and load the post, then look at the various command sections or G-code sections.

I was initially trained in UG/Post before PostBuilder exsisted.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[shags72]

You need to turn cutter comp on and make sure there is a D word in your linear move area. It usually is in there. You will have to mess around with the cc settings to get the G41 to come out where you want it but after you figure it out it won't be bad.

 

[Jaydenn]

Take a look at this picture.
It might help you.
This is my method to get cutcom to work. In your NX file, you activate it from the "Non-cutting moves", "More" tab.

One more thing to check... Open you operation in NX, Expand the "tool" tab, expand the "output" tab, make sure that the "CUTCOM" item has a check mark beside it.

For the I's and J's you simply go the the TOOLPATH > MOTION tab in post builder. Choose "Circular Move"

Drag the I, J and K items into the trash.

At the top of the window, there is a drop down. Go here and choose "R-Arc Raduis" from the "R" menu. Choose it and then press the "add word" button and drag it into the line. Thats it.

J

NX 6.0.5.3

 

[sitti]

I wanted to check my post process files, but I can find only tcl and def files. This way I think I can't open it in post builder.
Then I tried to create a new one, just to try, how it works. I selected Fanuc from the library, did some modifications, and saved it. I copied the files def, tcl, and pui, into the specified folder. Now I can see as an alternative in post process menu, but when I select it to make a program, I receive an error message.
Received an error 1770007
File name: o:\ugnx75\ip32\scr\camsmom\no\ind\mom_tcl_definitions.c, line number:1107
Error message: Cannot open file
C:\Program Fils\UGS\NX7.5\mach\resources\postprocessor\MV66A_Fanuc.tcl

Any idea what is wrong?

 

[markrief]

Did you add an entry to template_post.dat?


Mark Rief
Product Manager
Siemens PLM

 

[markrief]

I almost forgot...
Next time - try Tools --> Install NC Postprcessor.
It will copy all the related files to the correct location and add the new post to the list in the dialog.

Mark Rief
Product Manager
Siemens PLM

 

[moudy1]

After you get the error message select help from the main menu... NX log file... in the Information window scroll all the way to bottom then page up to the begining of the error section. It normally begins with ***TCL ERROR***. This will give you more information about what the problem is. It also helps when in postbuilder if you click on the Output Settings tab... other options... Check Display Verbose Error Messages.