[jgarner77]

Hi i hope i'm posting this in the right place as i've only just registered,I program and set 2 axis mori seiki and okuma and howa lathes (sl2,sl3 mori's and act-35 okuma's) all with fanuc controls 6t 10t the latest being 18t on the okuma's.I've never really used can cycles apart from G92 for threading and never use tnrc (G41/G42) either so therefore all our programs are always written with cad-cam knowing what inserts were using and making allowances for it when posting the program.Now i've finished waffling on having read manuals searched online i understand that G70/G71 assumes the radius of the tool is 0.0 so does that mean that my profile part of my can cycle should make allowances for my finish inserts radius i.e if im using a 0.8 radius insert programming a 2mm radius i should program it a 1.2 radius in my program and just accept that the roughing pass will be slightly out i hope this makes sense and hope theres someone who can advise me and if i've not come over clearly enough i'll try and explain more if anyone replies

Thanks in advance

[angelw]

Hi i hope i'm posting this in the right place as i've only just registered,I program and set 2 axis mori seiki and okuma and howa lathes (sl2,sl3 mori's and act-35 okuma's) all with fanuc controls 6t 10t the latest being 18t on the okuma's.I've never really used can cycles apart from G92 for threading and never use tnrc (G41/G42) either so therefore all our programs are always written with cad-cam knowing what inserts were using and making allowances for it when posting the program.Now i've finished waffling on having read manuals searched online i understand that G70/G71 assumes the radius of the tool is 0.0 so does that mean that my profile part of my can cycle should make allowances for my finish inserts radius i.e if im using a 0.8 radius insert programming a 2mm radius i should program it a 1.2 radius in my program and just accept that the roughing pass will be slightly out i hope this makes sense and hope theres someone who can advise me and if i've not come over clearly enough i'll try and explain more if anyone replies

Thanks in advance

There are some Fanuc controls that are able to accommodate the use of G41/G42 in the G71 roughing cycle and apply the TNR compensation correctly. However, "G70/G71 assumes the radius of the tool is 0.0" means that in the roughing cycle G71, tool nose radius compensation via the control is ignored, but it will be applied when the code describing the profile shape between and including the P and Q referenced blocks is executed using the finishing cycle G70.

If the OD profile shape has a monotonous increase in X, or an ID profile shape with a monotonous decrease in X, this will result in a "Metal On condition", and the part will not be ruined during the execution of the G71 cycle. However, if either profile shapes contain concave form, then the trailing edge of the insert will over cut the and probably ruin the part unless an extra large X finish allowance is used.

Personally, I don't care to use TNR compensation in turning operations, as unlike a machining centre where Cutter Radius Compensation is used to regulate the size of features being machined, lathes use the Geometry and Wear offsets for this purpose. By not using TNR compensation, none of the rules applying to its use have to be obeyed, and as the various intersection and tangent points of a profile have to be calculated whether TRN comp is used or not, its only a small further step to calculate the true location of the tool when manually creating the program, and no change in difficulty when generating the program via a CAM system. For me, the disadvantages of its use outweigh the advantages.

Regards,

Bill

[jgarner77]

Firstly thanks for your reply bill it is very much appreciated,I feel i am missing something as you say tool nose radius compensation will be ignored in a G71 block but executed in a G70 block how does the control know what radius of insert i'm using is there a table where i put it in or are you saying that if i program G41/G42 the G71 cycle wont read it and the G70 cycle will in which case i just need to program my finish pass between the p and q reference blocks allowing for the radius of my finishing insert and just accept that the G71 cycle will be slightly out is that correct

thanks again

[txcncman]

Tool size is entered in the machine control on the tool geometry screen.

[angelw]

Firstly thanks for your reply bill it is very much appreciated,I feel i am missing something as you say tool nose radius compensation will be ignored in a G71 block but executed in a G70 block how does the control know what radius of insert i'm using is there a table where i put it in or are you saying that if i program G41/G42 the G71 cycle wont read it and the G70 cycle will in which case i just need to program my finish pass between the p and q reference blocks allowing for the radius of my finishing insert and just accept that the G71 cycle will be slightly out is that correct

thanks again

In the Offset Registry pages of your control, where you are used to registering Geometry and Wear offsets, there will be another two columns dedicated to the Tool Nose Radius and the Number of the Imaginary Tool Nose of the tool being used. The Imaginary Tool Nose relates to the centre of the TNR, relative to the points on the TNR used when setting the Geometry Offsets of the tool as shown in the attached picture. The appropriate number associated with each Imaginary Tool Nose is registered in the Tool Type columns of the Offset being used with the particular tool. Similarly, the TNR of the tool is registered in the Tool Radius column for the appropriate offset number.

In your part program, when a tool change and offset call is executed, the values in the Tool Radius and Tool Type column for that offset being called become active and will be applied when G41 or G42 is used in the program. For example, if T0101 is executed, and 0.8mm TNR and Imaginary Tool Nose number 3 is registered in the corresponding 01 offset, then these two values will be used by the control to calculate the true tool location when G41 or G42 are used.

Although there are 8 Imaginary Tool Nose numbers shown in the attached pictures, all programming applications can be covered using numbers 2 and 3; it all comes down to the reference points of the TNR used when setting the tool. There are another two Imaginary Tool Nose numbers available, but are seldom used. They are 0 and 9, and are used when the centre point of the TNR is used as the reference when setting the tool.

i just need to program my finish pass between the p and q reference blocks allowing for the radius of my finishing insert and just accept that the G71 cycle will be slightly out is that correct

When using TNR compensation, you don't have to allow for the radius of the tool, the control does that; you just use the coordinates dimensions of the actual part. But you are correct in that the profile cut by the G71 cycle will be incorrect and made correct when the G70 cycle is executed. However, this will only work in this way if there are no concave forms in the profile as outlined in my previous Post. The other consideration is that the incorrect profile left by the roughing cycle may affect the deflective forces applied to the finishing tool, as the finishing allowance left won't necessarily be what you specify in the G71 cycle definition. There will be considerable more material left on tapered surfaces. The greater the angle of the taper, the greater the amount left. The greater the TNR, the greater the amount left on tapered surfaces.


Regards,

Bill

[jgarner77]

Thanks again for your advice guys and especially for pointing out the tool tip and radius columns and there meanings on the offset screen which i've always noticed but never (a) knew what they were for and (b) never needed to use them so that in itself is a triumph atleast but returning to my original problem as i think i might have mis-interpreted something along the way as i don't and never have used tnrc when programming everything is always programmed allowing for the radius of the insert by compensating my figures in the program so is that what i should do for my G71/G70 cycle just right my P Q reference lines to suit which ever radius of insert i plan to use for my finishing pass.So if i use a 1.2R tool to rough with then finish with a 0.8R should i just program it to suit the 0.8R tool

Thanks again for your advice really do appreciate it and hope i've made it clearer this time around

James

[txcncman]

Based on your last post, I would not program 2 separate tool paths, one for each tool. (Unless difficult cutting conditions called for it.) Just program for the finish tool radius like you indicated and let the roughing tool leave a little extra material in a few places. Normally this will not effect the outcome significantly.

[jgarner77]

Thanks guys thought that might have been the case just needed my theory backing up really thanks again for all your advice.

James