Hi All ,

I got troubles with the correction with this profile :

T2 M06
G00 X8. Z1. M08
G42
G01 Z0 F0.15
X10.2 K-0.6
Z-16.527
X9.6 Z-17.717
Z-17.9
X18. K-0.2
Z-27.
G40
X20. M09


the profile should looks like without correction , but with makes an strange undercut - anyone knows why ?
the tool is radius 0.4mm and tip 3.
__
Peter

I'm not sure I understand the K values in your code, but one thing to check is that you need to command an XZ point that is off the part profile at the end of the cut. This lead off point should probably be on the same line as the G40 command.

I understand the K-value being a incremental move forming a chamfer

but putting the G40 where it is is bad, it is cancelling the tool nose radius, and will gouge the part by whatever amount you have set in the comps page

As HuFlungDung says
Z-27.
G40 X20. F1.0
M09

Just make sure that the X-diameter move off the part is more than twice the tool nose radius.
G40 X19. F1.0 ( is the closest X for R0.4 tip )( tool moves X0.2 on the G40 line)

it is an outside profile , and my problem isn`t at the end of the profile , look at the photos, the first one is without the correction , and the part should look smillar to this , the second photo is with the G42 correction, and there is a problem, the third photo is a zoom to that place.

The pictures help

Seems to be a compensation error, your profile does not take into consideration of the R0.4 tip, run it thru using R0.0

If you have access to a CAD system, create the profile, offset this profile by 0.4, this is path the tool radius centre-point should be following,

It can't get to do the little taper ending at X9.6 before hitting the Z-17.717
wall

Adjust the u"cut profile to have a flat, that you know the tool tip will touch
or use a smaller tip radius

G01 Z0 F0.15
X10.2 K-0.6
Z-16.527
X9.4 (Z-17.717)
Z-17.9
X18. K-0.2
Z-27.
G40
X20. M09

You`re right , there was too small flat place there , I`ve made a mistake reading the undercut parameters by a 1mm , if I changed the point correctly then was OK .

Thanks for getting me on the right track.

__
Peter

Wielkie,

solved in 7 hours

Dopóki następnym razem

Wielkie,
solved in 7 hours
Dopóki następnym razem

was that on-line translated ? I don`t get the point. And not 7hours , I didn`t solved this at the time I was writing the post.

Don't we need a T0202 at the beginning to invoke the TNR?

Depends,
If you progran to the TNR centre, then you do not have to use T0202, as the value of the radius woud have to be zero.
on the other hand, you can program the path to "fudge" TNR in the profile, (as pit202 has done ) and then put TNR in the startup

TNR is not critical in facing or diameter turning, it is necessary on tapers and tightly toleranced radii

Sometime using TNR on a simple manually programmed profile can lead to thinning hair.

...Sometime using TNR on a simple manually programmed profile can lead to thinning hair.

Or big piles of it on the floor and head marks on the nearest concrete wall. :D

But once you have it sorted out it is so useful!!