This may seem like a moronic question but I'm just getting back into cnc's and programing. When you use cam software and it provides tool tip radius compensation do you still include the tool tip radius when you're setting up your turning tool geometry offsets. I don't want my parts to come out wrong because I didn't enter the radius value.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Tool tip compensation
- Thread starter bhaha
- Start date
- Replies 29
- Views 10,444
alexhawker
Aluminum
- Joined
- May 6, 2013
- Location
- Philadelphia, PA United States
Got a scrap of something laying around? Take a test cut and measure it?
Sent from my iPhone using Tapatalk
Sent from my iPhone using Tapatalk
gkoenig
Titanium
- Joined
- Mar 31, 2013
- Location
- Portland, OR
I'm like 4 months into owning a Robodrill, and programming it with SolidWorks/HSM Works...
I've never once input a tool diameter in the machine. All diameter compensation is done in CAM.
Having said that, there is an option in HSM Works to do diameter comp in CAM, but do tool wear comp in-machine... but I have not played with that yet to see how it actually works.
I've never once input a tool diameter in the machine. All diameter compensation is done in CAM.
Having said that, there is an option in HSM Works to do diameter comp in CAM, but do tool wear comp in-machine... but I have not played with that yet to see how it actually works.
Seems like my machine doesn't like when the program comes to an area that includes cutter comp. It alarms out which always sucks but I think that it's because I don't have a t value set and I don't know what that even is. A friend described it as how the tool was clocked but he couldn't remember what direction or numbers that are used. I do think that the tool tip being set in the offsets affects the size during cutter comp. The last cut I took this evening had the part way big when it should be on size. I think I'm going to just make the cutter comp adjustments myself and omit the command in the program. The cam software does some goofy stuff that is really starting to aggravate me.
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Hello bhaha,
When the Tool Radius Comp is included in the Tool Path by the CAM software, then generally, Tool Rad Comp is not used at the control. The Tool Radius can be set in the control, but will have no affect on the part being machined unless G41/G42 is made active via their inclusion in the Part Program.
There are two forms of Tool Radius Compensation that are generally used, Full and Partial:
1. In Full TRC, the tool path uses the actual geometry coordinates of the finished part, as if the tool being used has Zero Tool Nose Radius. In this case, the actual Tool Nose Radius of the Tool being used would be registered in the Tool Offset Registry of that tool and G41/G42 used in the Part Program to implement the effect of the TNR.
2. In Partial TRC, the Tool Path is created with the TRC included in the Part Program and G41/G42 also included in the Part Program. In this case, the Tool Radius registered in the Tool Offset Registry will be a small value and can be either side of Zero (+ or -). Partial TRC is more commonly applied in Milling rather than Turning applications.
Tool Rad Comp with a Machining Centre is almost admonitory, as that's the only method of sizing a feature when using the periphery of an end mill. This is not the case with a Turning Tool, where Tool Radius Comp is only required where Tapers, or Radii are involved and there the size of a diameter is regulated using the Position Offset of the tool and not generally the TNR Offset.
You will only get an alarm being raised by the control if TRC is being implemented at the control in response to G41/G42 being made active via the Part Program.
Regards,
Bill
HuFlungDung
Diamond
- Joined
- Jan 19, 2005
- Location
- Canada
What always caused me a lot of confusion when switching lathe programs between using toolnose rad comp or not, was in setting up the tool offsets themselves. For this reason, I always let the CAM do the compensation, then I never have to reset the tool offsets.
I might have missed something and am willing to be set straight, if anyone can point out what is wrong: if using TRC, then the tool datum lies at the arc center of the tip radius. So then, touching the tool off the work does not define the tool datum until you modify it by the amount of the tip radius. So, if you run with TNR off, then the tip is set too far into the work, so to prevent that, the final rough cut must always allow at least the amount of the tip radius for a following finish cut, or else the piece will be overcut at the roughing stage. (I do not use roughing or finishing cycles either, so ignore the effect when those are called up).
So then, if a guy makes a mixture of programs using the same tool set, but some calling for TNR comp, while others do not, then one must also remember to alter the tool offset datum by the tip radius, putting it in, or removing that amount. I think it becomes an unworkable nightmare, especially if your control will not allow you to assign a different offset register address than that assigned to the tool number (must match on my MITS).
I might have missed something and am willing to be set straight, if anyone can point out what is wrong: if using TRC, then the tool datum lies at the arc center of the tip radius. So then, touching the tool off the work does not define the tool datum until you modify it by the amount of the tip radius. So, if you run with TNR off, then the tip is set too far into the work, so to prevent that, the final rough cut must always allow at least the amount of the tip radius for a following finish cut, or else the piece will be overcut at the roughing stage. (I do not use roughing or finishing cycles either, so ignore the effect when those are called up).
So then, if a guy makes a mixture of programs using the same tool set, but some calling for TNR comp, while others do not, then one must also remember to alter the tool offset datum by the tip radius, putting it in, or removing that amount. I think it becomes an unworkable nightmare, especially if your control will not allow you to assign a different offset register address than that assigned to the tool number (must match on my MITS).
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Hello HuFlungDung,
This only applies if 0, or 9 are registered as the Tool Type and the tool set accordingly. Typically, Tool Type 3 and 2 will be used for a RH OD Turning Tool and RH Boring Bar respectively. In this case the Geometry Tool Offsets of the tool are established at the Leading Edge of the insert for Z and the part of the TNR that is closest to the machine centre line for X. Accordingly, there will be no difference whatsoever in the diameters and faces cut whether TRC via G41/G42 is used, or not. The only differences will occur on tapered and radius surfaces. Therefore, if two programs were prepared for the same component, one created with Tool Radius Comp calculated and included in the Part Program, the other created using the actual coordinate points of the finished part with TRC being applied at the control using G41/G42, then each program will machine parts to the same dimensions (within the accuracy of the machine), without any alteration of the Offsets, except of course, for tool wear.
Regards,
Bill
Last edited:
Ok so regardless of the tip radius my geometry offsets should show tool type as 3 for turning tools and 2 for boring bars. Should threading/grooving tools use the same tool type? Now as far as the TRC. With it in the program I shouldn't include tip radius in the geometry offsets, correct. But if it's not programed then the tip radius needs to be in the offsets. I think this is where I'm running into issues to some extent. The cam software doesn't post any cutter compensation until it's running a profile pass and that's usually when the brick wall shows up, but I haven't had the tool type entered into the machine either so I'm wondering if that's part of it too. None the less, the advice you guys have is very helpful.
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Hello bhaha,
Tool Radius Compensation is not used with a Threading Tool. The Profile of the Thread is generally formed with the shape of the Insert; its generally not a generated shape.
With regards to a Grooving Tool, whether TRC at the control using G41/42 were used would depend on the complexity of the groove profile and whether there were tapers and radii involved. If the profile of the groove was complex and it was decided to use TRC at the control, then effectively you're using two Tool Tip Types, type 3 when the front surface (closest to the chuck) is being profiled and type 4 when the rear surface is being profiled. In this case you would have to use Two Offsets for the one tool. For example, T0202 for the Leading Edge of the insert and T0222 for the Trailing Edge. In this case you could register Tool Tip Type 3 in offset 02 and Tool Tip Type 4 in offset 22. The compensation direction specified with G41/42 would be swapped when profiling the Front and Rear surfaces of the groove.
Just to make sure we are on the same page:
1. when I refer to TRC at the control, I mean that the tool path uses the actual coordinate points of the finished part and G41/42 is used in the program so that the control can compensate for the TNR of the Insert. In this case the Tool Tip Type and the Radius of the Insert being used must be registered in the Tool Offset Registry of the Tool being used.
2. when I refer to the TRC being included in the Part Program, I mean that the TNR of the Insert being used is compensated for when calculating the coordinates of the Tool Path. In this case, no G41/42 codes will be used in the program and therefore, it doesn't matter whether the Tool Tip Type and the TNR is registered, or not. If they are registered, they are not applied in any way if G41/42 is not executed in the program.
If when you say that your CAM software "doesn't post any cutter compensation until it's running a profile pass", you mean that G41/42 is not included in the program until the tool path is the actual profile of the part, then the Roughing should be carried out with the CAM software compensating for the TNR in the program.
With a R/H OD Turning Tool taking rough cuts on a profile, where the cutting motion is parallel to the Z axis and towards the chuck at the Left side of the machine, the Work-piece is to the left of the Tool Path and therefore, G42, compensation to the Right is used. When the tool reaches the end of the roughing pass, retracts from the work slightly and then Rapids back to the start point, the Work-piece is now to the right of the Path of the Tool. In this case, if G42 is still active, the control will compensate the tool to the Right of the Tool Path and unless the retract distance is at least twice the tool radius, the tool will interfere with the Work-piece. Therefore, unless your CAM software is able to determine change of tool direction and either cancel Tool Radius Comp, or swap to the opposite TRC mode (G42 to G41) at the appropriate time, this may be why Tool Radius Comp (G41/42) is not output in the Rough Operations.
If you mean that the CAM software is not calculating and including compensation for the TNR in the program, other than when Semi-finish, or Finish profiling, then I'd suggest that your CAM software is not configured correctly, or is Rubbish Software.
Even when hand programming for a lathe, I seldom use TRC at the control and particularly when CAM software is used, doing all the calculations for TRC, I never use it. As stated in an earlier Post, TRC for a Machining Centre when using End Mills is almost mandatory, as that's the only process by which the size of a feature can be regulated. With a lathe this is not the case. In my opinion, the biggest advantage when using TRC at the control (G41/G42 in the Part Program), is that a change in TNR can be made without having to re-post the Tool Path; all that is required is a change of the TNR registered in the Tool Offset registry for the particular tool.
Regards,
Bill
Last edited:
If your program does NOT have a G41/G42 then it doesn't matter what number is in the geometry offset page on the control for radius and tool tip number because it only reads those values when Cutter Comp is turned on.
HuFlungDung
Diamond
- Joined
- Jan 19, 2005
- Location
- Canada
To summarize my question in one point: when setting the tool offset by touching off the part, a different offset is used than when using TNR comp? The difference will be an X and Z adjustment equal to the TNR of the selected insert?
Hence, running a 'mixture' of programs, some calling for TNR comp and some that do not, will result in scrap parts if offset adjustments are not made (if you remember which the hell method they were set for
)
Hence, running a 'mixture' of programs, some calling for TNR comp and some that do not, will result in scrap parts if offset adjustments are not made (if you remember which the hell method they were set for
)No, set the tool normally.
If it was programmed with cutter comp, then you set it normally but input the insert radius on the offset page and the correct tool tip number 1-8 or 0-9 whatever it is, I only use 2 and 3.
If it was programmed without cutter comp BUT taking the insert radius into account, you set it normally and not worry about putting in the insert radius on the offset page.
Remember that TNR only really comes into play on angles and radii.
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
This thread is a perfect reason to use CAM and let it do it for you.
I don't think I have ever used comp for a tool tip on the lathe*, but I use only CAM. I suppose if you have a really tight radius or angle/taper it is needed...?
* Although I do need to have the tip direction/number to tell the probe how to set the tool in my Haas lathe.
I don't think I have ever used comp for a tool tip on the lathe*, but I use only CAM. I suppose if you have a really tight radius or angle/taper it is needed...?
* Although I do need to have the tip direction/number to tell the probe how to set the tool in my Haas lathe.
This thread is a perfect reason to use CAM and let it do it for you.
I don't think I have ever used comp for a tool tip on the lathe*, but I use only CAM. I suppose if you have a really tight radius or angle/taper it is needed...?
* Although I do need to have the tip direction/number to tell the probe how to set the tool in my Haas lathe.
I learned old school programming on a lathe. It was a Fanuc 0-T and didn't have conversation.
1/2 keyboard style and possibly my favorite part of a Fanuc control (and I hate Fanuc).
So I had to hand program all of my parts using cutter comp. I think it's something that every lathe programmer should learn almost immediately before going with conversation as it helps understand the breakdown of the program.
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
To summarize my question in one point: when setting the tool offset by touching off the part, a different offset is used than when using TNR comp? The difference will be an X and Z adjustment equal to the TNR of the selected insert?
Hence, running a 'mixture' of programs, some calling for TNR comp and some that do not, will result in scrap parts if offset adjustments are not made (if you remember which the hell method they were set for
Hello HuFlungDung,
No it doesn't. When G41/42 are made active in a program, the control uses Look Ahead blocks to calculate the True Position of the Tool to compensate for the effects of the TNR of the Insert.
In the attached picture, the Green Lines indicate the coordinate points at the Start and End of the Tapered Face. If you were to command the tool to position at the coordinate represented by the Bottom Right set of Green Lines, then the Tool Nose Radius of a R/H OD Turning Tool would locate to where the Bottom Right Red Circle (Tool Nose of Insert) is shown. This is based on the normal setting of a R/H OD Turning Tool where the Leading Edge of the Insert is set for Z and the point of the TNR closest to the machine centre line is set for X. If the program were to execute a Linear Interpolation move to the coordinates represented by the Top Left set of Green Lines, then the Tool Nose Radius of a R/H OD Turning Tool would locate to where the Top Left Right Red Circle (TNR) is shown.
In making a Linear move from the location of the Bottom Right Red Circle (TNR) to the location of the Top Left Red Circle (TNR), then the Tool Nose Radius would move along the Red Line shown. The Grey Line represents the True Surface of the Work-piece. Accordingly, when the actual coordinates of the Work-piece are used in the Part Program and no TRC is used at the control by making G41/42 active, in the example of the tapered surface shown, an amount of material represented by the distance between the Red and Grey parallel lines will be left on the Work-piece.
The Yellow Circles represent the location of the TNR at the Start and End of the Tapered Surface, when:
1. the actual coordinates of the Work-piece are used in the Part Program and when TRC at the control is used by making G42 active.
2. the coordinates used in the Part Program have been calculated to compensate for the TNR of the tool being used. In this case, TRC at the control by making G42 active will NOT be used. If a TNR value and a Tool Tip Type have been registered for the Tool, they will be ignored when G41 and G42 are not active.
In the case of 1 and 2 above, the Yellow Tool Nose Radius would move along the Grey (True Surface of the Taper)
Therefore, when the Geometry Offset of a tool has been correctly set, the tool can be used with equal success in a program where TRC at the control is used (G41/42 included in the Part Program)and in programs where the Tool Compensation has been calculated and included in the coordinate values used in the Part Program and where TRC at the control is NOT used (no G41/42 applied in the Part Program). This is an example of the same Tool, using the same set of Offsets can be used in the one program in the one overall machining operation, where the part is machined with TRC turned off for some features (the Face) and on for others.
In a Work-piece where the end of the part (Z Zero - Face Perpendicular to Z axis) is faced, it is profoundly typical for TRC to be cancelled (G40), as the position of the TNR will be the same with, or without TRC active. TRC would then be made active by executing G42 when the tool is moved to the Start of the Taper.
In summary, the same tool, with the same Offset can be used to machine a Work-piece with, or without TRC being active, provided that the coordinates in the part program accommodate the use of, or not, Tool Radius Comp at the control. There will be no scrapping of parts due to the same set of Offsets being used for programs with and without TRC being calculated by the control.
Regards,
Bill
WayneC369
Hot Rolled
- Joined
- Jan 4, 2014
- Location
- ATL, GA, USA
Hi Bill,
I think the picture below taken from a Fanuc Manual illustrates what you are saying. Please correct if need be. My question is, based on your statement above, does the control actually compensate just prior to the rapid (G00) retract to the starting position (assuming G71 cycle is in effect)? Therefore, if using a cutter with an unusually large radius, i.e. 8mm round RCMT, there is a potential for the cutter to contact the chuck jaws should enough clearance not be allowed?
Thanks,
Wayne
On the controls I've programmed, there is no cutter comp in a G71 cycle, only the G70 finish cycle.
And I'm pretty sure the control compensates ON the G00 move off the part since my controls can't have G41/G42 on during a rapid move.
How I've always programmed my parts:
G00G40X2.5Z.1
G01G42X2.F.012
Z0.
X2.2Z-.1
Z-2.
X2.3
G00G40X10.Z10.
M30
WayneC369
Hot Rolled
- Joined
- Jan 4, 2014
- Location
- ATL, GA, USA
Hmmmmm...... something for me to ponder. I am new to CNC turning, so my intent is not to argue with those in the know. I am still hammering out my methods and programming style/format. I have found what works, at least on this Fanuc 18TA, is I issue a G42 during the rapid move to the starting position of a G71 cycle, run the cycle, then later call a G70 using the same technique, i.e. TNRC prior to calling the G70. Whether this is proper programming or not I'm unclear, but the control doesn't complain and the parts turn out the way I want them. I'm sure I'm missing something that will bite me later.
So, do you think the control drops the TNRC prior to entering the G71 cycle?
HuFlungDung
Diamond
- Joined
- Jan 19, 2005
- Location
- Canada
I appreciate what you are trying to explain, and I am not trying to be obtuse here
When I am reading through a program on the control, I want the program to show the exact diameters that are being turned (supposing the path has no tapers and no radii) Hence I would write the exact same finish path coordinates, whether or not I used TNR comp. I don't want to read diameters that are OD + 2x tip radius just because I am not using TNR comp, because it gets too confusing. I gather from what you wrote, that you are writing two different finish paths, depending on whether you intend to use comp, or not. Is that how you do it?
Edit: trying to clarify my issue here: if I machine a given path with no rad comp on in the control, and then go and add the tip radius, and modify the program to turn on G41/G42, then run the same path again on the same part in the machine, the tool will 'cut air' with comp active. It will follow a parallel path, displaced by the tip radius amount above the part.
(my point is to stick with one system or the other: no TNR comp at the control for any programs, or, all programs use TNR comp. All programs are written finish part path exactly).
