Why i don´t get rapid feed between the holes

[Arnold]

Hello,

what do i wrong. The G-Code between holes goes up and down. After this he moves slowly to the next hole.

I´m using FreeCad 0,18 16093 for Windows

[sliptonic]

It looks like you selected the top face for profile and then set the depth down to the bottom.

If, instead, you select the cylindrical faces for all the holes, you'll get rapid moves between them

[RatonLaveur]

Hello Arnold, hello sliptonic,

First of all, thanks for answering Arnold, I was in the process of giving him the same answer yesterday after fiddling with his file

Knowing your colossal contribution to Path, perhaps you'll be able to enlighten me: I understand that machining different faces automatically generates rapids in-between, that's the way Path operates (and most machines in the industry anyway because time is $$$), but is there a specific reason the drilling operation generates regular feed rates in-between features?

Thank you!

Jerry.

[herbk]

Hi Jerry,

The moves between the holes are allways rapid moves, it's part of G81 command.

http://linuxcnc.org/docs/2.7/html/gcode ... #gcode:g81

and

http://linuxcnc.org/docs/2.7/html/gcode ... ary-motion

[RatonLaveur]

Hi herbk,

Thank you for helping, I tested Arnold's code and if you do what he did:

- "Select" [top face] --> "Select" [Profile Based on Faces] --> "tick" [Process Holes], then the result is as he describes it. The cavities (hole, inner rectangle) are processed correctly but the travel in-between cavities is G1, so normal feed rate.
This leads to no G81 command, and the moves have no reason even through linuxcnc to become G0 (unless i'm mistaken).

If you instead do what sliptonic adequately pointed out:

- "Select" [inner faces of holes] --> "Select" [Profile Based on Faces], then the result is the same machining path but with rapid retracts and rapid moves. As Arnold wants it.

Of course if you instead "Select" [ inner faces of holes]--> "Select" [Create a path drilling object from a feature...], then the drills are G81 and path assumes you've selected the right tool for the job (i.e. in this case, not a single 4 mm end-mill, otherwise your result might be interesting )

From my understanding, it's because Path will generate rapids in-between discrete areas.
Since the base feature in the initial approach by Arnold is a single face, there is no instruction for Path to perform rapids.

My question to sliptonic is out of curiosity: is that a voluntary feature or simply that "tick" [Process Holes] is not yet coded to generate rapids.

[sliptonic]

My question to sliptonic is out of curiosity: is that a voluntary feature or simply that "tick" [Process Holes] is not yet coded to generate rapids.

It's a bug. At least it's an unintended consequence of the way the operation is coded. I'd love to see it fixed but since there's an adequate work-around, it will probably be a low priority issue.

Please feel free to open a ticket for it in Mantis. It might be a great place for someone to cut their teeth working on Path.

[RatonLaveur]

Thank you. I'll consider getting a Mantis account. Since I'm so new here I try not to "pester" with requests and help when I can.

After pushing a little more the limits of the [Profile based on face] on Arnold's file and making a quick file for myself, I am now convinced that there is something amiss here...and I think i've found it!

Hereafter from his own file:

Screencap one: Facing operation based on top face with "holes" ticked and the same parameters he requests (finaldepth -5.0 mm and stepdown 0.5mm): The processing seems perfectly fine.

Screencap two: Now, as Arnold did in his file, I put "Use Start Point" to True. Then the rapids are removed.

This is the limit of my understanding at the moment however.

[rainharvester]

I tried the workaround, but I can't get rapid feeds. (v 0.18)

I have some holes. I select the inner faces of the holes. I select "profile based on face or faces". Then I click tickbox "process holes".(later, I also tried not ticking).
I have the "SetupSheet" set for "Horiz Rapid" 12mm/s. And "Vert Rapid" = 12mm/s. (later I typed these directly into the tool parameters, but no luck).
But those values don't ever make it to the gcode.

I tried "Helix" too. I tried changing the Job's "Output" to grbl-G81, grbl, and centroid.

Am I doing something wrong?
What exactly is the workaround?
In this pic, only the "F540" is seen. Never do I get any rapid "F720".

[IMback!]

Ill look into this while changing freecad Tavel behaviour, so soon.