Peck Drilling with a dwell on each peck

[Roger]

I'm drilling some deep holes in 304 SS, 6.75" deep, with a .5" HSS drill.  The drill tip is taking a beating.  I ran across this article https://www.practicalmachinist.com/vb/cnc-machining/peck-drilling-151128/  so I thought doing it with a dwell might help.

This is on a Haas mill, And I don't know if it would support this.  Would this be a custom drill cycle?  If so, how can I implement this?  Post mod?

[Chally72]

Yes, this would be a custom cycle, as Haas G83 peck drilling only supports a dwell on the last peck. If it's only a few holes, just do a normal G82 drill cycle with a dwell, and copy and paste the operation a few times and set the depths successively deeper. Then at least you can try the dwell at each peck without writing out a long form cycle. By the way, I have read the same thread you posted and used the knowledge within for stainless and Inconel. It helps. I was doing more damage with IPT feeds too slow than I was with not having a dwell- just some advice.

Another tip for saving the tip, if you will, in stainless- use a 142° spot drill and not a center drill to spot the hole location! Too few people do this.

[Roger]

1 minute ago, Chally72 said:

Yes, this would be a custom cycle, as Haas G83 peck drilling only supports a dwell on the last peck. If it's only a few holes, just do a normal G82 drill cycle with a dwell, and copy and paste the operation a few times and set the depths successively deeper. Then at least you can try the dwell at each peck without writing out a long form cycle. By the way, I have read the same thread you posted and used the knowledge within for stainless and Inconel. It helps. I was doing more damage with IPT feeds too slow than I was with not having a dwell- just some advice.

Thanks, Chally72.  What kind of speeds and feeds do you recommend?  I've been using 70 SFM in 304 using HSS tooling, and my feed on this job is .003 FPT., with .1 peck.

[Chally72]

That would vary wildly by tool. I always skip over HSS and use cobalt. Just as a guess, your SFM might be too high for HSS. I go all the way down to 18SFM in some stainless parts to get the best drill life and hole quality on low quantity parts. Also, don't drop down to a 0.1" peck until you're deeper in the hole. Only peck when you need to in order to eke more life out of that drill!

[gms1]

Sometimes if i have a drill cycle that doesn't fit any of my current options I just make it a point to point program and use change at point to get it to do what i want. This just makes it a bunch of g0/g1 commands instead of a canned cycle.

[Roger]

7 minutes ago, gms1 said:

Sometimes if i have a drill cycle that doesn't fit any of my current options I just make it a point to point program and use change at point to get it to do what i want. This just makes it a bunch of g0/g1 commands instead of a canned cycle.

This job is now done.  Your idea sounds very interesting!  Could you post an example of this?

[gms1]

T28(7/32 MZE DRILL)
M06
G54G17G90
G00A0.B0.
M161(SPINDLE CLAMP ON)
X.3969Y-2.8602S1100M03T1
G43H28Z.05
M08
G94G01Z-.08F4.
G00Z.05
G01Z-.35F4.5
G00Z-.32
G01Z-.65
G00Z-.62
G01Z-.85
G00Z.05

So this is the output code for one of my parts that use this. You could easily add in some g4 dwell commands at any one of these points to get your dwell how you want. Inside mastercam you use the point toolpath and it looks like this for me:

 

 

I just individually select each point and tell mastercam whether it is a rapid or feed move. then I edit the commands to get the feed rates I want or add in whatever i need from there. There are some limitations but this is the basics of it.

If I do something really oddball there are times where I will just insert a manual comment with all the codes I need for a toolpath if it doesn't fit into anything available.

[Roger]

THANKS!  I'll give that a try next time.   After programing for 18+ years I'm still learning!  This forum is the best! 

[crazy^millman]

1 hour ago, gms1 said:

T28(7/32 MZE DRILL)
M06
G54G17G90
G00A0.B0.
M161(SPINDLE CLAMP ON)
X.3969Y-2.8602S1100M03T1
G43H28Z.05
M08
G94G01Z-.08F4.
G00Z.05
G01Z-.35F4.5
G00Z-.32
G01Z-.65
G00Z-.62
G01Z-.85
G00Z.05

So this is the output code for one of my parts that use this. You could easily add in some g4 dwell commands at any one of these points to get your dwell how you want. Inside mastercam you use the point toolpath and it looks like this for me:

 

 

I just individually select each point and tell mastercam whether it is a rapid or feed move. then I edit the commands to get the feed rates I want or add in whatever i need from there. There are some limitations but this is the basics of it.

If I do something really oddball there are times where I will just insert a manual comment with all the codes I need for a toolpath if it doesn't fit into anything available.

With toolpath editor and cantext you can edit the feedrates and also add dwells at each point.

[Roger]

7 minutes ago, C^Millman said:

With toolpath editor and cantext you can edit the feedrates and also add dwells at each point.

I have never used cantext before.  When you say "with toolpath editor"  what do you mean???  Can you explain more for this naïve programmer? 

[crazy^millman]

Well it pretty much goes like this. You have to have changed your Cantext to support the G4 dwell. If you did then you would get that output when called here I am just taking the standard MPFAN and showing you with like the example above how you can use the toolpath editor to change feed and rapid moves. This works on any Mastercam toolpath and I have used this as long as I have used Mastercam.

PDF link to the Screen shots showing how to do the process

 

 

 

 

Edited August 20, 2020 by crazy^millman
Pictures removed to save space

[crazy^millman]

DP

 

 

 

 

Edited June 26, 2018 by C^Millman
Double Post no reason to repeat myself.

[Roger]

20 minutes ago, C^Millman said:

Well it pretty much goes like this. You have to have changed your Cantext to support the G4 dwell. If you did then you would get that output when called here I am just taking the standard MPFAN and showing you with like the example above how you can use the toolpath editor to change feed and rapid moves. This works on any Mastercam toolpath and I have used this as long as I have used Mastercam.

I will experiment with this, when I get a slow day.  LOL!!!  Thanks for taking the time to do up this example!

[jlw™]

1 hour ago, C^Millman said:

Well it pretty much goes like this. You have to have changed your Cantext to support the G4 dwell. If you did then you would get that output when called here I am just taking the standard MPFAN and showing you with like the example above how you can use the toolpath editor to change feed and rapid moves. This works on any Mastercam toolpath and I have used this as long as I have used Mastercam.

I couldn't tell you how many times I've used this since Ron showed it to me.

[crazy^millman]

5 minutes ago, jlw™ said:

I couldn't tell you how many times I've used this since Ron showed it to me.

Thank you glad to know I am helping others.

[gms1]

I always know that at the end of the day there will always be another way to accomplish what I did that day in mastercam. Its all about time and effort management. And usually I have 0 time to do anything

[Roger]

19 hours ago, gms1 said:

Its all about time and effort management. And usually I have 0 time to do anything

DITTO HERE!!