Drilling without using a cycle

[RACINGCONVERTERS]

Is there a way to change from using a G81 drill cycle to a point to point drilling. (not using cycle syntax)

[gms1]

There are ways to do that. You can do a point to point toolpath, You can have your post output long hand code so its all g1/g0. You can also use advanced drill and that would get you g1.

[Guest]

8 minutes ago, RACINGCONVERTERS said:

Is there a way to change from using a G81 drill cycle to a point to point drilling. (not using cycle syntax)

Depending on your post, usually you can disable drill cycles in the control definition page.

I think the section is called drilling cycles.

[RACINGCONVERTERS]

I was able to adjust the post to not post the cycle. Thank You for the help.

 

One more question! Is there a way to change to post fast feed instead of rapid?

[Guest]

13 minutes ago, RACINGCONVERTERS said:

I was able to adjust the post to not post the cycle. Thank You for the help.

 

One more question! Is there a way to change to post fast feed instead of rapid?

That's usually set in the operation parameters, uncheck "rapid retract"

[RACINGCONVERTERS]

That option is greys out in the drill toolpath I have.

[Guest]

Which operation?

[RACINGCONVERTERS]

Drilling cycle

[Aaron Eberhard]

Probably not..  A "regular" G81 cycle specifies that it rapids out, so unless you mod your post to not output rapids, it most likely will exit with a rapid.   Perhaps the advanced drill will do what you need?  That one doesn't rapid out, but has a feed retract rate.

[crazy^millman]

Why not use a G85 cycle?

[Guest]

On 3/5/2021 at 5:04 PM, Aaron Eberhard - CNC Software said:

Probably not..  A "regular" G81 cycle specifies that it rapids out, so unless you mod your post to not output rapids, it most likely will exit with a rapid.   Perhaps the advanced drill will do what you need?  That one doesn't rapid out, but has a feed retract rate.

The op has drilling cycles disabled..

Does that change the outcome?

[Colin Gilchrist]

11 minutes ago, Thee Byte™ said:

The op has drilling cycles disabled..

Does that change the outcome?

Not really. The movement output is G0/G1. 
However, there is a "convert rapid to feed" switch in the CD. This does need to be incorporated into your Post, to get the G1 Fxxx. For Rapid moves.

To get this to work, it is really Post Dependent.

[gcode]

On 3/4/2021 at 1:31 PM, RACINGCONVERTERS said:

I was able to adjust the post to not post the cycle. Thank You for the help.

 

One more question! Is there a way to change to post fast feed instead of rapid?

Try the Rapid page of the Control Definition

There is an option there to force G01 rapid mtion

The go to the Machine Definition and define the MAX rapid speed.

This will not work if you are using a really old post that does not respect the Machine/Control definitions

[RACINGCONVERTERS]

Following the steps from GCode seems to have worked like I wanted.  

I have been looking for the advanced drill cycle,  I have yet to find it or how to find the advanced features of the drilling.  Can anyone point me in the right direction on that, to further my knowledge.

[gcode]

41 minutes ago, RACINGCONVERTERS said:

I have been looking for the advanced drill cycle,

Advanced Drill is new to MC2021

If your siggy is accurate, you don't have it 

[RACINGCONVERTERS]

Thank you GCode.  I am using 2020 currently.  I can upgrade I just haven't.

 

I should probably change my siggy.