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:

Changing drill speed mid cycle


JB7280
 Share

Recommended Posts

For the part I'm working on, I'm forced to use some uncomfortably long aircraft drills.  (.257D, with 8.375" out of the holder) and I'm getting a bad finish.  Drill manufacturer recommends starting at slow RPM, and kicking the rpm up once it's in engaged (unfortunately, due to other features, I'm not able to pilot the hole, but i AM spotting.)  Is there a way to do this in my mastercam file, or will I need to write a manual entry??

Link to comment
Share on other sites

For 2020 and before, I would do this with driving the drill around with Point toolpath to make RPM/speed changes mid-hole where I wanted to.

For 2021, there's a new Advanced Drill toolpath that allows you to build your own custom drill cycle, segment by segment, and individually control coolant settings, RPM, feed, peck settings, and manual entry and comment insertion for each segment. Post output is not canned cycle, but easily readable G1/G0 movement that in our testing works very well with existing posts.

I know I've responded with 2021 plugs on the last three posts now, but there's an avalanche of new toys that I've been using nonstop here in Applications.

Link to comment
Share on other sites
4 minutes ago, Chally72 said:

For 2020 and before, I would do this with driving the drill around with Point toolpath to make RPM/speed changes mid-hole where I wanted to.

For 2021, there's a new Advanced Drill toolpath that allows you to build your own custom drill cycle, segment by segment, and individually control coolant settings, RPM, feed, peck settings, and manual entry and comment insertion for each segment. Post output is not canned cycle, but easily readable G1/G0 movement that in our testing works very well with existing posts.

I know I've responded with 2021 plugs on the last three posts now, but there's an avalanche of new toys that I've been using nonstop here in Applications.

How would I do that with points?  Or at least somewhere to start so I can figure it out?

Link to comment
Share on other sites

Attached is a file with an Iscar 0.630 self centering drill being driven by a point to point toolpath (Operations 13-16) to drill holes with no spotting in the angled faces of this part. We needed to come in with a slow feed until we hit full diameter engagement, then change the feedrate to drill the rest of the hole. The green wireframe you see there is what I drew to provide the necessary Z points for each change in feed or other parameters that I wanted to make.

Here's a link to a video of the part being cut- skip to 1:20 for the angled face drilling: https://www.youtube.com/watch?v=KlV-tqUrlIM

 

Let me know if you have any questions!

DEMO PART 1018.mcam

  • Like 2
Link to comment
Share on other sites
1 hour ago, Chally72 said:

Attached is a file with an Iscar 0.630 self centering drill being driven by a point to point toolpath (Operations 13-16) to drill holes with no spotting in the angled faces of this part. We needed to come in with a slow feed until we hit full diameter engagement, then change the feedrate to drill the rest of the hole. The green wireframe you see there is what I drew to provide the necessary Z points for each change in feed or other parameters that I wanted to make.

Here's a link to a video of the part being cut- skip to 1:20 for the angled face drilling: https://www.youtube.com/watch?v=KlV-tqUrlIM

 

Let me know if you have any questions!

DEMO PART 1018.mcam

So, each change in feed or rpm requires a new toolpath?  or am i looking at this wrong?

 

Link to comment
Share on other sites
23 minutes ago, JB7280 said:

So, each change in feed or rpm requires a new toolpath?  or am i looking at this wrong?

 

You can actually string together multiple points in the Point toolpath, but for ease of readability and edits if ever coming back to the file, I split it out into individual toolpath segments.

Link to comment
Share on other sites
13 minutes ago, nickbe10 said:

That's 30+D.

Generally piloting should start at 9D for best results.

 

8 minutes ago, The Chipmaker said:

  I would start with a short drill the same diameter at first at least 3x dia. Reference this thread from a couple of weeks ago. Pretty much like Chally72 said. Hope this helps!

 


I understand that, however, as i said in the original post, there's just no option for that on this part.  the hole is up against a wall, 7.8" high, that allows for a max diameter of .310.  Figure in .030" casting variance, and bobs yer uncle.

Link to comment
Share on other sites
50 minutes ago, JB7280 said:

 


I understand that, however, as i said in the original post, there's just no option for that on this part.  the hole is up against a wall, 7.8" high, that allows for a max diameter of .310.  Figure in .030" casting variance, and bobs yer uncle. 

What options are there about smacking the design engineer around a bit with a large trout?

  • Like 2
  • Haha 4
Link to comment
Share on other sites

The actual issue with the hole is that when you put a pin in, and shine a light through, you see 3 points touching the pin.  Inside the hole it almost looks smeared, with dark spots, and I think i'm able to see a spiral score, like one that would be caused by the drill dragging on retract.  Drill manufacturer suggested higher RPM, but do you think that would actually fix it?  Or should I just get an extended length reamer to finish the holes, and call it a day?

  • Like 1
Link to comment
Share on other sites
28 minutes ago, JB7280 said:

The actual issue with the hole is that when you put a pin in, and shine a light through, you see 3 points touching the pin.  Inside the hole it almost looks smeared, with dark spots, and I think i'm able to see a spiral score, like one that would be caused by the drill dragging on retract.  Drill manufacturer suggested higher RPM, but do you think that would actually fix it?  Or should I just get an extended length reamer to finish the holes, and call it a day?

is the hole blind or through? Can it be drilled from the other side?

Link to comment
Share on other sites

If it is dragging there is a drilling cycle that turns off the spindle at the bottom of the holes.The hollow shape could give you more vibration if you increase your speed too much, so if you are keen on drilling maybe decrease your peck size.

If you arent aiming for precision a reamer is overkill.

Link to comment
Share on other sites
14 minutes ago, Peter from S.C.C.C. said:

If it is dragging there is a drilling cycle that turns off the spindle at the bottom of the holes.The hollow shape could give you more vibration if you increase your speed too much, so if you are keen on drilling maybe decrease your peck size.

If you arent aiming for precision a reamer is overkill.

I'm not pecking.  I tried a peck and the condition didn't change.  Also tried G85 (feed in, feed out) and G86 (spindle off, rapid out) boring cycles, same condition.  I agree, a reamer is overkill for the tolerance, but if I can't get the form/finish.....

23 minutes ago, AHarrison1 said:

is the hole blind or through? Can it be drilled from the other side?

They are through, but other feature block entry from the other side.  I'm actually drilling from both sides.  The length is required either way.

Link to comment
Share on other sites
2 hours ago, JB7280 said:

I understand that, however, as i said in the original post, there's just no option for that on this part.  the hole is up against a wall, 7.8" high, that allows for a max diameter of .310.  Figure in .030" casting variance, and bobs yer uncle.

I situations like that I always like to request that they move the hole closer to the wall just for the challenge. That usually gets them going...not necessarily in a helpful way...what's the material?

Link to comment
Share on other sites
40 minutes ago, JB7280 said:

I'm not pecking.  I tried a peck and the condition didn't change.  Also tried G85 (feed in, feed out) and G86 (spindle off, rapid out) boring cycles, same condition.  I agree, a reamer is overkill for the tolerance, but if I can't get the form/finish.....

Yeah, if you need it, you need it, Imo if u do a small peck like .005 to .01" it should yield a good finish and clear the chips.

Link to comment
Share on other sites
27 minutes ago, nickbe10 said:

I situations like that I always like to request that they move the hole closer to the wall just for the challenge. That usually gets them going...not necessarily in a helpful way...what's the material?

A356-T6 cast AL

IMG_20200401_164616.jpg

Link to comment
Share on other sites
1 hour ago, 5th Axis CGI said:

Try drilling undersize and then get a endmill ground to size and chase the hole with an endmill. Cast Aluminum can present these challenges.

The issue there, is that it would be have to be a .257, 9 inch long endmill, lol, I'm not sure if that would create any better of a finish.  You think??

 

The gentleman from the tool manufacturer suggested I remove the spot, since the drill is faceted, and enter at about 600 rpm, and .002"-.003" per rev, then ramp up to 2200rpm once the full diameter is engaged.  Do you think that's going to give me any better results?  2200 seems high for such a long drill, even if it is already engaged.

 

Not spotting also seems crazy with a 8.375" stickout, on a cast surface.

Link to comment
Share on other sites
1 minute ago, JB7280 said:

The gentleman from the tool manufacturer suggested I remove the spot, since the drill is faceted, and enter at about 600 rpm, and .002"-.003" per rev, then tamp up to 2200rpm once the full diameter is engaged.

Maybe it is a lot, but the cutting speed for that material is very high.. I would try it. Maybe close the door lol.

3 minutes ago, JB7280 said:

9 inch long endmill,

If you have a welder, you could weld one onto some  drill rod, I have seen it before, it worked I suppose.

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...