Feed Plane Overwriting Rapid Plane V26

I am drilling holes with a rapid plane of 2" to clear some clamps. I have my feed plane at .1 because i don't want to be feeding air for two inches. However when the tool path is computed the drill rapids to .1 from hole to hole. I changed the posted code from G99 to 98 so it will hopefully work. But how do i get the computed toolpath to rapid to 2" and feed at .1? Thank you.

Quote:

---

Originally Posted by Jbrown74

I am drilling holes with a rapid plane of 2" to clear some clamps. I have my feed plane at .1 because i don't want to be feeding air for two inches. However when the tool path is computed the drill rapids to .1 from hole to hole. I changed the posted code from G99 to 98 so it will hopefully work. But how do i get the computed toolpath to rapid to 2" and feed at .1? Thank you.

---

It is the G98/G99 setting that is causing the behavior you describe. You may have to edit your PP to make sure it only uses G98. I don't know your particular machine but if I program a G99 in any drill cycle, the tool will only return to the "R" plane before moving to the next hole. G98 will force the tool to return to the Rapid plane, move to the next hole, then rapid down to the R plane.

In the V26 software for drilling the Rapid Plane Value is the Initial Plane Value. And the Feed Plane Value is the Retract Value for the Drilling Canned Cycles. If you are long coding these then they would be rapid and feed panes


MikeG

I guess I will just have to change the G99 to G98 manually, does anyone know how to make it automatically post to G98? Thank you for the clarification MikeTheG.

Quote:

---

Originally Posted by Jbrown74

I guess I will just have to change the G99 to G98 manually, does anyone know how to make it automatically post to G98? Thank you for the clarification MikeTheG.

---

Try opening your PP in Notepad and look for the lines that control the G98/G99 output shown below :-

515. Output G99 instead of G98 in drilling? y
516. Output G98/G99 in drilling? y

I believe changing the "y" to "n" in line 515 should do it.

Remember just "Save" the PP after modifying, do not do a "Save as" or the PP will just be saved as a txt file and not a MillPst file.

Regards
Rob
:rainfro: :rainfro: :rainfro:

Thanks a lot Engine, the computed tool path is still off but at least I don't have to manually changed the code every time. And the predator backplot seems to be running the correct path.

PS how do you save as to MILLPST. I want a copy for safe keeping.

Well, if you " copy" the file, it would be a millpst file, and just rename it. But, might I warn you, I think you should never modify your actual post, I only modify a copy of the post, and after proving out that no unintended change have occured, then I will save the new edited post as my day to day post. Just my opinion