Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
-
Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!
tool register default output 2
- Thread starter Jaydenn
- Start date
Depending on how your post-processors are set up, Cutcom and Adjust values equal the tool number on post-processing. Cutcom defines a cutter radius or diameter offset, (depending on how it's defined in your machine controller tool tables), Adjust defines the G43 H value.
e.g. T6 M6
G90 G21 G0 G54 X100. Y-100. S15000 M3
G43 H6 D6 Z50. M8
However, you can have your post-processor configured such that you can output independent H and D values thus.
T6 M6
G90 G21 G0 G54 X100. Y-100. S15000 M3
G43 H6 D56 Z50. M8
Using Cutcom allows some flexibility with regard to tool usage, particularly with machines with limited tool pockets.
For example, let's say you wanted to use tool number 6 for some open limit milling like a rough slot, your cutter radius D register number, (used during cutter compensation paths G41 or G42 in Fanuc code) would equal 6. However, if you wanted to use the same tool later on in the machining process, say to machine a finely toleranced bore diameter feature, you assign a different Cutcom number in order to output the different D register value, (in this example D56). The effect of this in machining land is that you can edit your wear compensation value 56 in the machine tool table to tweak your bore diameter on the fine machining, without affecting the slot width on the first feature.
I hope that's an adequate description.
e.g. T6 M6
G90 G21 G0 G54 X100. Y-100. S15000 M3
G43 H6 D6 Z50. M8
However, you can have your post-processor configured such that you can output independent H and D values thus.
T6 M6
G90 G21 G0 G54 X100. Y-100. S15000 M3
G43 H6 D56 Z50. M8
Using Cutcom allows some flexibility with regard to tool usage, particularly with machines with limited tool pockets.
For example, let's say you wanted to use tool number 6 for some open limit milling like a rough slot, your cutter radius D register number, (used during cutter compensation paths G41 or G42 in Fanuc code) would equal 6. However, if you wanted to use the same tool later on in the machining process, say to machine a finely toleranced bore diameter feature, you assign a different Cutcom number in order to output the different D register value, (in this example D56). The effect of this in machining land is that you can edit your wear compensation value 56 in the machine tool table to tweak your bore diameter on the fine machining, without affecting the slot width on the first feature.
I hope that's an adequate description.
- Thread starter
- #6
Moog2,
The post processor will output these values by default.
Unless of course, your post has been altered in some way to remove them.
It's simply a matter of turning on the output (the item this thread is based on...)
and turning cutcom on in the operation. Go to the "NON CUTTING MOVES" dialog and choose the "MORE" tab. You will see the cutcom options.
Turn it on and post! see what happens.
Keep in mind that most machines CANNOT apply D-comp on an arc. You will get CRC alarms on the control.
Be sure the "G41" or "G42" appear on an X Y linear move.
J
The post processor will output these values by default.
Unless of course, your post has been altered in some way to remove them.
It's simply a matter of turning on the output (the item this thread is based on...)
and turning cutcom on in the operation. Go to the "NON CUTTING MOVES" dialog and choose the "MORE" tab. You will see the cutcom options.
Turn it on and post! see what happens.
Keep in mind that most machines CANNOT apply D-comp on an arc. You will get CRC alarms on the control.
Be sure the "G41" or "G42" appear on an X Y linear move.
J
- Thread starter
- #7
Hi, I need to resurrect this question.
I have still been unable to get this check box to be default "on".
Bert, what do you mean by change the template file...
I am using my own template, but there is no setting that I can see to change the option. Thats the problem.
Thanks,
J
I have still been unable to get this check box to be default "on".
Bert, what do you mean by change the template file...
I am using my own template, but there is no setting that I can see to change the option. Thats the problem.
Thanks,
J
You should be able to open your template.
Lock the Cutcom to Inherited and save the file
Restart NX - this is the quickest way
Reload Your template and the change should be there.
John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO
NX3,4,5,6 Solid Works, Pro/e, Solid Edge
Lock the Cutcom to Inherited and save the file
Restart NX - this is the quickest way
Reload Your template and the change should be there.
John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO
NX3,4,5,6 Solid Works, Pro/e, Solid Edge
- Thread starter
- #9
John,
It's not the "inherited" setting that's the problem...
It's the physical checkmark.
Whenever I make an operation, the "Value" for the cutcom is there (inherited from tool) but the check box to output it is UN CHECKED.
If I don't remember to check it, the information is NOT passed to the post processor.
Really annoying.
J
It's not the "inherited" setting that's the problem...
It's the physical checkmark.
Whenever I make an operation, the "Value" for the cutcom is there (inherited from tool) but the check box to output it is UN CHECKED.
If I don't remember to check it, the information is NOT passed to the post processor.
Really annoying.
J
-
2
- #10
I am familiar with this problem, and fixed it in NX 7.0.
The problem is that the cutcom register output toggle does not turn on automatically when the value is inherited. Once this toggle has been turned off in the operation, it stops inheriting, and it will not turn on by itself again, and there is no UI to turn the inheritance back on. This is why turning it on in the template does not work - it still will not be inherited.
You can fix your parts in NX6 by running the attached vb program - rename it from .txt to .vb.
This will correct the situation in all operations in the work part. I recommend you also open each template part, such as mill_planar.prt, run the program, and save the part, to prevent future problems.
Mark Rief
Product Manager
Siemens PLM
The problem is that the cutcom register output toggle does not turn on automatically when the value is inherited. Once this toggle has been turned off in the operation, it stops inheriting, and it will not turn on by itself again, and there is no UI to turn the inheritance back on. This is why turning it on in the template does not work - it still will not be inherited.
You can fix your parts in NX6 by running the attached vb program - rename it from .txt to .vb.
This will correct the situation in all operations in the work part. I recommend you also open each template part, such as mill_planar.prt, run the program, and save the part, to prevent future problems.
Mark Rief
Product Manager
Siemens PLM
Download the program.
Rename the extension to .vb.
Open the template part mach/resource/template_part/metric/mill_planar.prt.
Go to Tools --> Journal --> Play, Browse, pick the file, and Run.
Save the part.
Repeat for each template part that you use.
Mark Rief
Product Manager
Siemens PLM
Rename the extension to .vb.
Open the template part mach/resource/template_part/metric/mill_planar.prt.
Go to Tools --> Journal --> Play, Browse, pick the file, and Run.
Save the part.
Repeat for each template part that you use.
Mark Rief
Product Manager
Siemens PLM
- Status
Similar threads
- Locked
- Question
- Locked
- Question
- Locked
- Question