Dolphin Turn - Mach 3 - Don't want TNRC output

[Chris D]

Hi everyone,

I am new to Dolphin - love it so far. I am using it with Mach 3 turn and am about to run my first real part. I am trying various posts to see which works closest with Mach 3.

The biggest issue I have right now is to force Dophin to NOT output G41/G42/G40 for profile turning. I would rather have Dolphin perform the TNRC compensation.

Does anyone have any suggestions as to how I can do this?

BTW, the nearest match for a MACH 3 post is F3t (of the ones tested so far).

Thanks

Chris

[andre-dolphin]

Hello Chris,

Tool comp ! the one topic that everyone has different views on. Here's how PartMaster deals with it - this is the same for Milling or Turning, Wire EDM is slightly different as this needs to done on the machine tool.

Area clear operations - No tool comp is applied at all, all moves generated are for the tool diameter specified in when the tool is defined.

Profile Turn - Turning and Goround - Milling the same rules apply to both.

The default method is for PM to use the tool radius and offset the toolpath accordingly, this allows us to check for undercuts and re-entrants and prevent overcutting, the tool radius register in the controller should be set to zero as normally no further offsetting is required, however it's often the case that certain amount of fine tuning may be required at the machine tool, for instance you cut the part and when it's measured it's over/under size. This is why the post processor outputs G41/G42 to allow you to input a small value into the radius offset register to compensate for over/under sizes and re-cut the part. If you really dont want the G41/G42 then the post needs to be altered, I think there may already be one from Steve B. If not it's an easy change.

The alternative method is to use what is referred to as "Part Surface Programming" this is switched on/off from the Options tab in Profile Turn or Goround. The effect of this is that the tool radius value IS NOT taken into account when creating the toolpath. Instead the coordinates output are that for the surface of the part. In this instance the tool radius must be set correctly on the machine tool. This of course can be modified to take into account over/under sizes. BUT and it's a BIG BUT --- PM will not even try to look for undercuts and /or over cutting, it's then down to you to make sure the part can be cut with the tools you are using. This a far more important for Turning than Milling as it's quite easy to see where a round tool will fit. In Turning we not only account for the tool tip radius but ALSO the tool geometery angles.

The recommended methos is for PM to take care of tool offsetting as it's always better that the machine tool.

Hope this as clear.

ATB
Andre

[Chris D]

Hi Andre,

Thanks for responding. To clarify further....

I too believe that it would be best for part master to handle the tool nose radius compensation. Seldom if ever is the radius of the insert changes on the tool once a job is programmed which eliminates the need for the user to input tool nose radius information at the control.

Furthermore, TNRC (G41, G42) is NOT needed on a lathe control for part size adjustments. This is handled by the wear offsets which are selected with the tool code (in most cases) such as T0303. T0303 selects tool 3 offset 3. Wear offsets are not associated to G41 and G42.

I asked Steve B. on another group if he has a post for MACH Turn - hopefully he does which will save me a bit of effort to eliminate the output of G41/G42. If not, I will try to turn it off in the post - I just have not looked in there much yet.

Thanks again

Chris