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

17 hours ago, JB7280 said:

A356-T6 cast AL

I just can't imagine keeping a stable cut going on a high aspect ratio like that at much more then 500 - 600 rpm (probably less) until you have at least 1.5D engaged.

What kind of drill are you using, have you tried Guhring Technical guys? Carbide or HSCo? I have seen long shank and relatively short flute length drills which might be a little more rigid if you can get them in that size.

Have you dialed in the drill like a reamer? 

If you drop the spot drill you will almost certainly need to make a flat on the cast surface.

Holes are nothing but misery, my mentor used to assure me. 

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

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.

No I don't think you will have a problem with getting a surface finish. Speed and feed is everything with the right speeds and feed you can machine anything. I have hung tools our 40XD and machined features just comes down to the correct speed and feed. Look to a 3 Flute drill they don't need to be spotted and you have tons of room around that part so not sure why you haven't looked at an ER-11 or something help strengthen the tool, but since we don't have a full picture hard to know exactly what will help.

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

No I don't think you will have a problem with getting a surface finish. Speed and feed is everything with the right speeds and feed you can machine anything. I have hung tools our 40XD and machined features just comes down to the correct speed and feed. Look to a 3 Flute drill they don't need to be spotted and you have tons of room around that part so not sure why you haven't looked at an ER-11 or something help strengthen the tool, but since we don't have a full picture hard to know exactly what will help.

That picture is one of the holes in the pattern.  The others have very little clearance.  Nothing larger than .312 diameter will fit due to a tall "chimney" type feature next to the holes.  Unfortunately I can't share a picture of the part.  

 

1 hour ago, nickbe10 said:

I just can't imagine keeping a stable cut going on a high aspect ratio like that at much more then 500 - 600 rpm (probably less) until you have at least 1.5D engaged.

What kind of drill are you using, have you tried Guhring Technical guys? Carbide or HSCo? I have seen long shank and relatively short flute length drills which might be a little more rigid if you can get them in that size.

Have you dialed in the drill like a reamer? 

If you drop the spot drill you will almost certainly need to make a flat on the cast surface.

Holes are nothing but misery, my mentor used to assure me. 

I am using a 12" long, HSS/Carbide Tip Aircraft drill from CJT Koolcarb.  I have dialed in the drill, I was actually surprised at how straight these drills are.  About .0005" runout at the tip before I even tweaked it.  Less than .0002" now.   The drills are as you said, Long shank, relatively short flute length.  I'm beginning to think it may just be the material that is to blame.  I've got a reamer on the way.  I took about 75% of the cycle time out of this part, and numerous secondary operations, so i guess we can spare a little time for the reamer.

  • Like 2
Link to comment
Share on other sites
8 minutes ago, JB7280 said:

I am using a 12" long, HSS/Carbide Tip Aircraft drill from CJT Koolcarb. 

You might want to try Guhring, those guys have got me out of trouble on things like this. Although modern carbide is "sharper" than in days of yore, HSS can still be sharpened to a finer edge which might give you easier penetration, they do some long split point and parabolic tips that might help you out here. The carbide is more rigid, to be sure, but it just might not be the best compromise here. You are definitely "out of the boat" so be open minded (you seem to be that already).

The "3 point" appearance is not unlike the holes you can make in sheet if you use a drill point that penetrates the far side before picking up the full diameter so the chip doesn't form properly, this could also be caused by the point building up pressure before finally it penetrates the surface. But now again your chip formation is not "timed" properly.

If the HSCO can penetrated more freely then the stability might be maintained,  if you can balance the tool pressure with the helical effect. It might also broaden out your machining parameter "window", which will be relatively narrow whatever you come up with.

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

You might want to try Guhring, those guys have got me out of trouble on things like this. Although modern carbide is "sharper" than in days of yore, HSS can still be sharpened to a finer edge which might give you easier penetration, they do some long split point and parabolic tips that might help you out here. The carbide is more rigid, to be sure, but it just might not be the best compromise here. You are definitely "out of the boat" so be open minded (you seem to be that already).

The "3 point" appearance is not unlike the holes you can make in sheet if you use a drill point that penetrates the far side before picking up the full diameter so the chip doesn't form properly, this could also be caused by the point building up pressure before finally it penetrates the surface. But now again your chip formation is not "timed" properly.

If the HSCO can penetrated more freely then the stability might be maintained,  if you can balance the tool pressure with the helical effect. It might also broaden out your machining parameter "window", which will be relatively narrow whatever you come up with.

I didn't know that guhring deals in aircraft drills. I'll contact them.  Thanks

Link to comment
Share on other sites

In an effort to use what's in house, for the time being, I found a homemade drill extension, and put a HSS screw machine drill in, and the holes came out round.  Although, same crappy finish.  I'm pretty certain at this point that the finish is a product of the casting.  This is a long term part, so I'm hesitant to use a shop built drill extension, so I just may end up getting a drawing on file with a tool grinder for a long drill with a slightly larger shank.  thanks for the help!!

  • 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...