Spotting & drilling down inside

[StoneyNH]

Im working on a part that has alotta tapped holes down at Z-.640.How can I get the spot & drill to rapid down to Z-.640 before executing its move?Right now after every move it rapids up to Z .050 & feeds down to Z - .640 which wastes alotta time.I cant use G98 cuz theres islands in the way.Is there a way to get the tools to rapid down to Z-.640,do its move,rapid up to Z .050,then rapid down to Z-.64 again?

[duckdogers]

I would put the retract at -.590

[Guyinthedesert]

G0 G90 X? Y?

G43 H? Z.05

G98 G81 Z-? R-.64 F?

G80

 

 

Will that not do what you want?

[specv]

Im confuzed, this is exactly what G98 is for, inital plane Z.05 R plane -.590

 

G99 would not work if there are islands as it would rapid to the R plane to move to the next hole.

[Thad]

Use an incremental retract of .1 and an incremental top of stock of 0. Select the top of the hole as your geometry (assuming you have a top and bottom of the hole).

[duckdogers]

if clearance is set at .05,retract at -.590 it should work.I never have it rapid down to start point(in this case -.64

[The Cathedral]

Set top of stock to -.640

Set retract to .05, incremental

Set clearance to .05, absolute, make sure box is NOT check to only use at start and end.

[StoneyNH]

I tried T.O.S. @ -.640,retract .05 incremental,clearance .05 absolute with start & end unchecked

I get G99 G81 Z-.675 R-.59 F13.

I cant have that because I have numerous islands in the way.

I guess I should mention Im using  2D graphics.

[Oscar R.]

I tried T.O.S. @ -.640,retract .05 incremental,clearance .05 absolute with start & end unchecked

I get G99 G81 Z-.675 R-.59 F13.

I cant have that because I have numerous islands in the way.

I guess I should mention Im using  2D graphics.

Your retract and clearance numbers can not be the same. Change your clearance number to something above what you have entered in your retract, doesn't have to be much just different. This will give you what your looking for.

[StoneyNH]

retract is .05 Incremental,clearance is .050 absolute,so the numerical values the same but theres different types,i tried changing the clearance to .060,got the same results

 

G99 G81 Z-.675 R-.59.

 

Am I attempting something that just cant be done?

[specv]

what is your top of stock set at?

[MikronGuy]

Clearance set to Absolute      1.00

Retract set to Incremental        .05

Top Of Stock set to Absolute  -.64

Depth set to absolute              -????????

If your drill cycle is set correct the tool will start at Z1.00, rapid to Z-.59 to start drilling to programmed depth, after drilling tool will retract to Z1.00 then move to the next hole clearing the islands on the part rapid down to Z-.59 and start all over.

 

The key is the clearance plane value. I know a lot of programmers that do not use that feature.

[specv]

set your retract to a -.590 absolute

[StoneyNH]

micron guy,you know what im trying to get,ill try what you suggest.can you give an example of what the G codes will look like?

[The Cathedral]

If you've tried what the others have suggested and it's not working, the problem lies within your post or machine definition. I do G98 and G99 drill day in and day out and it's always worked the way I need it to. Since we're all telling you pretty much the same thing and you're still not getting results, you've got to dig deeper.

[StoneyNH]

specv I tried -.590 absolute retract,gives me the same thing,G99 G81 Z-.675 R-.59,so its no good,I have islands in the way at Z-.050

[StoneyNH]

Cathedral,I utilize G98 or G99 when milling pockets or contours & it works good.

 

But this is drilling so its different.

 

Can you give me a G code line of what Im trying to do looks like?

 

Im attempting to rapid down to T.O.S. execute my feed in,rapid up above my islands,move to next position,rapid down to T.O.S. & feed in

[specv]

i am getting

G43 H1 Z.05

G98 G81 Z-.64 R-.59 when I use these settings:

 

clearance: .05 absolute

retract: -.59 absolute

top of stock: 0 incremental

depth: -.64 absolute

[The Cathedral]

N2 ( ISCAR .610" SUMO DRILL )
G0 G40 G80 G90 G54 P1 S1000 M3
G43 H2 X-2.0607 Y1.4774 Z.05 M8
G98 G81 Z-1.5 R-.59 F5.
X-1.633 Y-.3577
X.8865 Y.7465
X2.0062 Y-1.3219
X-.0855 Y-1.8274
G80
M9
M5

[The Cathedral]

Cathedral,I utilize G98 or G99 when milling pockets or contours & it works good.

 

But this is drilling so its different.

 

Can you give me a G code line of what Im trying to do looks like?

 

Im attempting to rapid down to T.O.S. execute my feed in,rapid up above my islands,move to next position,rapid down to T.O.S. & feed in

 

MIlling pockets and drilling is two completely different animals inside the brain of mastercam and in the post. Just because it works in milling, that has no affect on the drilling cycles. It's very possible your drill cycles weren't configured right, and no matter what you do all you'll get is a G99.

[StoneyNH]

Cathedral,so what youre telling me is all I have to do is change my G99 to a G98? I could do that manually.But then the tool is still going to retract to Z-.59 isn't it?

[Guyinthedesert]

Cathedral,so what youre telling me is all I have to do is change my G99 to a G98? I could do that manually.But then the tool is still going to retract to Z-.59 isn't it?

No, your tool will retract to the clearance plane, which is wherever the Z is at the start of the cycle. (ie G43 z???)

That is the whole point of G98

 

Go to your control def, under machine cycles choose return to initial height

[Oscar R.]

If it has worked for you in the past with the same machine definition and post, then it most likely that there's something wrong with your process. But if this is something that your just know trying with this machine definition and post than what Cathedral said here in his last post is very possible.

 

If you do not know how to work on your post or machine definition I would recommend contacting your reseller to help solve this.

 

Like Cathedral said, milling and drill are two different animals as far as the post goes.

[StoneyNH]

It sure sounds like whoever edited my post did something wrong.Im going to try simply changing my G99 to a G98 & see what happens.

[mikenaturalice]

Hmm... I can't say anything that hasn't been said but I will put my perspective on it.

G98= return to initial Z, for example if you program G43 H1 Z5. G98 G81 Z-.65 R-.5 your drill will rapid from the 5. to what your R value is and then rapid back up to the 5. (which would be over the top of your islands) then move to the next position. 

G99= return to R plane, so if your code is G43 H1 Z5. G99 G81 Z-.65 R-.5 it will rapid to and from the R value of -.5 (which would crash into your islands) then rapid to the next positon.

 

I have seen this before where another Z value before the drill cycle gets posted so that becomes the initial which can cause problems like this - 

G43 H1 Z5.

Z.1 <-- this has now become the initial Z value which will screw you up if you are thinking it will rapid back to the 5.

G98 G81 Z-.65 R-.5