G81 drill weirdness in MC

[roland27]

Hi

 

I was doing some drill operations, and found a problem with the post export. I tried the new post from the site here, and though the code format is changed, the core problem isnt.

 

Basically, a simple validation program here is to drill 3 full depth holes, and a partial depth 4th hole. Then a tool change, followed by a full depth pass at the 4th hole.

 

The problem is, on line 200 the post is inserting a G80 prior to the move on 210, so the partial depth drill is happening at the 3rd hole coordinate.

 

Am I missing something here? Why would MC want to place a G80 before the 4th hole is drilled, assuming this is not required to update the Z depth prior to the drill? And shouldnt it implement a G1 prior to the next move, assuming the G80 is needed for some reason?

 

As I mentioned, this happens with the generic Fanuc3 mill PP, and also the updated PP from the site here.

 

Regards,

Roland

 

N100G00G17G20G40G80G90

N110T104M06( 1/4 DRILL)

N120(MAX - Z.1)

N130(MIN - Z-.8)

N140G00G17G90G54X-1.25Y0.S1069M03

N150G43H104Z.1

N160G94

N170G99G81Z-.8R.1F4.28

N180X1.25

N190X.315Y-1.5945

N200G80

N210X-.5762Y-1.5873

N220G99G81Z-.3R.1F4.28

N230G80

N240M05

N250G91G28Z0.

N260M01

N270T10M06( NO. 76 DRILL)

N280(MAX - Z.1)

N290(MIN - Z-.8)

N300G00G17G90G54X-.5762Y-1.5873S1800M03

N310G43H10Z.1

N320G94

N330G99G81Z-.8R.1F4.28

N340G80

N350M05

N360G91G28Z0.

N370G28X0.Y0.

N380G90

N390M30

[Midwest]

Try Inc. for your drill depths not abs.

 

 

You can then drill all your holes at different depths (If you want) in one operation.

 

 

HTH

[roland27]

Very interesting workaround. Im not sure if/how the incremental component is involved here though. If I do just select all 4 points for a G81 cycle, and then later go in via Geometry and select the final hole (and do Change at Point/Depth) that eliminates the offending G80.

 

Is there a simpler way to manage this (using incremental- ie a list of depths by hole, etc)?

 

Either way- this is a great workaround- thanks so much.

 

Still wondering why MC is inserting that G80 though-

 

Best,

R

[Midwest]

quote:

---

then later go in via Geometry and select the final hole

---

This is not what I mean.

 

You can do when you are picking your holes If they are drawn in 3d mode and you use Inc.

 

 

HTH

[Guest]

+1 Midwest,

 

This can be accomplished by placing the points at the depths you actually want to drill depth to be and then picking all points and setting the depth to INC.

[Guest CNC Apps Guy 1]

quote:

---

...Very interesting workaround...

---

A workaround implies there is a bug. This is no bug. It's a lack of understanding in how mastercam figures depths of features.

[roland27]

I am a software developer by training. In that world, a bug is an error in code. A workaround is an alternate process allowing a desired outcome to be realized if the primary process is not effective. The alternate process suggested by Midwest is a workaround. My followup to his workaround is the question- 'is there a bug either in the NCI generation or in the PP that is inserting a G80 command mid-81?' If the system is inserting a G80 mid-process in a single drill operation, and not implementing a G0/1 prior to the next move, so far as I can tell- this is a bug. If this is not a bug, perhaps you could let me know why a G80 is placed where I believe it shuold not be- so we can all understand how Mastercam figures depths of features?

 

Regards,

R

[Midwest]

quote:

---

The alternate process suggested by Midwest is a workaround.

---

How long have you used Mastercam????????

 

This is NOT a work around.

 

Maybe put your file on the FTP

 

Someone will help you..........or try reading the Mastercam help files. This really is an easy and fast way to drill holes at different depths.

[Midwest]

quote:

---

A workaround implies there is a bug. This is no bug. It's a lack of understanding in how mastercam figures depths of features.

---

+1000

 

 

[Guest]

quote:

---

How long have you used Mastercam????????

---

My guess, 'bout 10 minutes

 

[Midwest]

Member Number: 18307

Registered: 09-01-2007

Posts: 3

 

 

Welcome to the forum roland27

 

 

[Guest CNC Apps Guy 1]

quote:

---

..A workaround is an alternate process allowing a desired outcome to be realized if the primary process is not effective...

---

Provided the primary process was the correct one that should have been used in the first place.

 

quote:

---

...The alternate process suggested by Midwest is a workaround...

---

Ummmmm, no. Should have been the primary process because of multiple depths being needed in the same toolpath operation. Basic training in the operation of the software would have identified that.

 

 

Now for some explanation...

G0 is modal and was active before the canned cycle was called. So any move after the G80 is a rapid/positioning move. Though technically there are G1 moves in the caned cycles, practically(what the control sees in this instance) there are not. Thatt's the machine side of the explanation. The Mastercam side of the explanation as to why a G80 is issued when a different depth is called has to do with how the cycle works in the Post. There's two sections at work in the post, the actual cycle call for the first point and the subsequent points section. I'm guessing (since I've not really dissected with a fine tooth comb the drilling cycles in a long time) if a difference in Z is detetectd it will issue a cancel drill cycle and initiate it again for the remaining hole(s).

 

HTH and welcome to the forum.

[roland27]

Apps Guy-

 

Yes, that helps a lot. I appreciate the insight. I still am missing something- which is 'why' if MC issues a G80 it would not call a G0 or G1 prior to the next drill op. Regardless, if this is how MC does things- now I know. What is a bit confusing is that in the Verify mode, MC indicated the original process as valid- with the partial depth drill on hole 4, followed by the full depth drill with tool #2. On the mill, different story. Yes, I am very new to MC guys (learning on a friend's station on weekends)- and if this is all trivial, OK. But if the process I initially defined is invalid, Verify sure didnt seem to mind. There are a whole lot of posts on various CNC forums about 'buggy' G81 processes in MC, and so I think perhaps there is some general confusion out there even among people who are not total newbies

 

Cheers all-

R

[roland27]

Oh, one clarification though Apps-

 

The initial process was not a single toolpath operation. It was 3- (1) the full depth drill operation on 3 holes, (2) the partial depth drill on the 4th hole, and (3) the toolchange/full depth drill on the 4th hole. Maybe that helps explain why Im a little more lost than a normal newbie;) Each operation machine as anticipated if selected/posted independently, but if all operations are posted at once, operation 2 behaves differently on the mill.

 

Regards,

R

[Guest CNC Apps Guy 1]

quote:

---

...I still am missing something- which is 'why' if MC issues a G80 it would not call a G0 or G1 prior to the next drill op...

---

It does not need to. The machine condition (universally I believe) is still pratically in a G00 mode and once the canned cycle is completed (after the G80 is read) so it's unnecessary for Mastercam to issue a G0. If any need it, it would only be the very old controls.

 

{quote]...'buggy' G81 processes in MC.... Hmmmm gonna need to look into that.

[doyleg]

roland27, your program looks and works perfectly on our machines. as midwest had stated, if you don't want the g80, have the initial drilling cycle set to incremental and pick the geometry for your 4 holes from the hole depth that you want. not from the top. Now you don't need the second op. You will only need the next op with the no 76 drill.

 

as it is. again, your program is good. If it doesn't run right, it's in your machine control, you may need to tweak your post to output the g0's.

[heavychevy2155]

I alway go change the drill depths in the operations manager. I select my drill path, then select the geo. tab, then choose the point I want to change, right click, then change at point and adjust the depth, hit ok and regen. It posts out perfect everytime, I'll have a XY and Z output for every drill depth change, and get a G80 at the end of the toolpath.