Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Advanced Drill - Wow. Finally. This is awesome!


Colin Gilchrist
 Share

Recommended Posts

I'm playing around with 2021.

Here is output from the 'Advanced Drill' Toolpath. This was generated with "MPFAN.PST". (No Post Edits Required!!!)

I produced this output with a 'single toolpath in Mastercam'.

Color me impressed...

%
O0000(T)
(DATE=DD-MM-YY - 21-01-20 TIME=HH:MM - 16:29)
(MCAM FILE - T)
(NC FILE - \\SELWAYSBS2K8\USERS\CGILCHRIST\MY DOCUMENTS\MY MASTERCAM 2021\MASTERCAM\MILL\NC\T.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T62 |  1/8 DRILL | H62 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T62 M6
N130 G0 G90 G54 X-1.7896 Y.5023 A0. S200 M3
N140 G43 H62 Z5.
N150 Z.1
N160 M5
N170 S200 M4
N180 G4 P2.
N190 G1 Z.25 F300.
N200 G4 P2.
N210 G1 Z-.375 F80.
N220 M5
N230 S200 M4
N240 M88
N250 G4 P3.
N260 G1 Z-.4 F5.
N270 S500 M4
N280 G4 P.5
N290 G1 Z-.41
N300 G4 P.5
N310 S2000 M4
N320 G4 P.5
N330 G1 Z-.42
N340 S4800 M4
N350 G4 P2.5
N360 G1 Z-.43
N370 G4 P2.
N380 G1 Z-.93 F28.
N390 G0 Z-.89
N400 G1 Z-1.43 F28.
N410 G0 Z-1.39
N420 G1 Z-1.93 F28.
N430 G0 Z-1.89
N440 G1 Z-2.43 F28.
N450 G0 Z-2.39
N460 G1 Z-2.93 F28.
N470 G0 Z-2.89
N480 G1 Z-3.43 F28.
N490 G0 Z-3.39
N500 G1 Z-3.93 F28.
N510 G0 Z-3.89
N520 G1 Z-4.43 F28.
N530 G0 Z-4.39
N540 G1 Z-5. F28.
N550 G0 Z-4.96
N560 M5
N570 M09
N580 G4 P3.
N590 G1 Z-5. F0.
N600 S200 M4
N610 G4 P2.
N620 M5
N630 G0 Z5.
N640 M5
N650 G91 G28 Z0.
N660 G28 X0. Y0. A0.
N670 M30
%

 

  • Like 5
Link to comment
Share on other sites
1 hour ago, c++ said:

Looks good Colin , is this a *new operation?

Yes, brand-new. 

And so sorely needed. I've written many "deep-hole drill cycles" (custom cycles), and it is always a pain. The UI for a custom cycle is really hard to use, and requires you to manually enter a bunch of numbers in different locations. This Advanced Drill path gives us a table of 'drill segments', which are all customizable. 

  • Like 3
Link to comment
Share on other sites
1 minute ago, Colin Gilchrist said:

Yes, brand-new. 

And so sorely needed. I've written many "deep-hole drill cycles" (custom cycles), and it is always a pain. The UI for a custom cycle is really hard to use, and requires you to manually enter a bunch of numbers in different locations. This Advanced Drill path gives us a table of 'drill segments', which are all customizable. 

Yes, this is very good for deep hole drilling, I can't sah that I have ever tried the custom cycles but I will take your word for it that it is complicated. I can't wait to hear more of what's new! Drill is only one of the areas where mastercam needs some work. Would be nice to see some enhancements in FBM toolpaths and Nesting. Also would like to see osciliatilon motion in pocket toolpath.

Link to comment
Share on other sites

This is fantastic news. As we manufacture hydraulic manifolds, these parts contain hundreds of drillings and reamings. To speed things up, many custom cycles have been created (such as multifeed/spindle cycle which is similar to the stuff above, but extremely restricted due to limited parameter count). I have already reached the limit on custom cycles. It is especially frustrating that you cannot link custom parameter to feature. I truly hope the new operation allows associativity between drilling depths and points.

13 hours ago, Colin Gilchrist said:

And so sorely needed. I've written many "deep-hole drill cycles" (custom cycles), and it is always a pain. The UI for a custom cycle is really hard to use, and requires you to manually enter a bunch of numbers in different locations. This Advanced Drill path gives us a table of 'drill segments', which are all customizable. 

I couldn't agree more. I skipped 2020 altogether because of all the negative feedback and hope CNC emphasized refining basic things with 2021.

Link to comment
Share on other sites

This is a great improvement.  I would still like to see when you do a 2D contour, the option to "peck" the endmill into the material if there isn't an entry hole. Instead of using a slow plunge feed.   Maybe have the option in the depth cuts page.  Back in my Surfcam days, I used that option all the time.  Then switched to Mastercam when i changed jobs, and really miss that option.

  • Like 2
Link to comment
Share on other sites
36 minutes ago, navsENG said:

So I may not have to hand program gun drills anymore?? 

My re-seller wrote me a lovely gundrilling cycle - it'll be on the forum somewhere. By memory it was based on Pinkys one (that definitely is on here somewhere) and i'd tweaked/buggered about with it and my reseller polished it to do exactly as i wanted.

 

  • Thanks 1
  • Like 2
Link to comment
Share on other sites
3 hours ago, SlaveCam said:

I skipped 2020 altogether because of all the negative feedback

You can't let random internet strangers dictate your decisions. 

No matter the product, there will ALWAYS be people that are unhappy with it.

Someone could cure all forms of cancer tomorrow and people will still post negative feedback on it for some reason or another.

  • Like 2
Link to comment
Share on other sites
56 minutes ago, cncworker said:

but, can you add a "peck" cycle?  So the tool pecks like a drill before doing the contour.

You can use the "entry drill" function to analyze the entry point of each "plunge point" for the Toolpaths you select. 

This creates a separate "Drill Op", before the "selected ops", which you can use to Peck Drill (with the endmill).

Link to comment
Share on other sites
2 minutes ago, Aaron Eberhard - CNC Software said:

Glad you like it, guys :)

Colin, I think we already have the "switching back to a M3 after a M4" thing in progress, but would you mind send your file in to QC so Jamie can  add it to the defect and we can verify that it's fixed as soon as the story is done?


Thanks!

Happy to Aaron!

It would be wonderful eventually if we could click on a "solid or surface" that is cylindrical, and have those be associated to a "segment" in the interface. 

 

Link to comment
Share on other sites
36 minutes ago, Colin Gilchrist said:

Happy to Aaron!

It would be wonderful eventually if we could click on a "solid or surface" that is cylindrical, and have those be associated to a "segment" in the interface.  

 

Thanks mate!

We're probably not going to go that direction per se, because that would be a lot of jumping in and out and weird dependencies and kind of annoying in reality, I think.   Look for future enhancements to this toolpath to start leaning more on extracting data from a defined hole...

Link to comment
Share on other sites

I currently do a lot of deep holes with large spade drills

Spade drills like to explode if the breakout is an angled surface ..

so I drill them to near breakout with the spade drill then finish the breakout with a high speed cobalt drill

Step 1 Point tool path … slow rpm .. rapid to hole's r plane feed to bottom of  hole at a fast federate  F20-F30

Step 2 G83 drill cycle .. rpm to cutting speed and peck drill a break through hole

Step 3 a point toolpath  slow the rpm and fast feed out of the hole

It would be awesome if this new drill toolpath could let me do that with one toolpath

entry

call up a canned cycle

then exit

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...