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:

Helix bore feedrates and rough pitch


chipman
 Share

Recommended Posts

Chipman always look to what the manufacture say is the ramp angle the endmill will allow and then go from there. I always like to stay below the recommend chip angle. A lot of it comes down to experience and also what you are going to be cutting. Aluminum I get crazy with it since as long as the tool is moving it is cutting, then go to some 55RC I go the opposite direction and get cautious. Rule of thumb for me is what would be my depth of cut on the endmill and then how much area do I have ot allow that to happen. 1/8 endmill going into a .15 hole not much room need to take it easy. 3/4 endmill going into a 1.25 hole I do it differently. Other factors are do I have thru the spindle coolant, is it high pressure or regular? Are you using a 2,3,4,5,8 or 10 flute endmill. Is it solid carbide end mil or an inserted endmill? Rules are funny things in my book yes I am glad we have them to follow, but sometimes you just to pay attention to what your machine, tool, set-up and material are telling you. A good programmer goes out to the machine and learns from the machine as much as they learn from the program. I pay attention to the chips, the cutter and everything else and make a mental note okay that worked or that failed. Yes we all have failed yes I got my share of mistakes and yes my hum should have not done that moments.

  • Like 1
Link to comment
Share on other sites

Crazy,

Thanks for the input, the whole rough pitch field in helical bore seems broken, it should allow angles.

That said I think I have to quit using the helix bore and start using contour with ramp. it has the angle field option.

The only advantage to helical bore is that it uses the point selection option which helps when selecting many holes.

With the contour option I have to manually chain each hole.

Link to comment
Share on other sites

Crazy,

Thanks for the input, the whole rough pitch field in helical bore seems broken, it should allow angles.

That said I think I have to quit using the helix bore and start using contour with ramp. it has the angle field option.

The only advantage to helical bore is that it uses the point selection option which helps when selecting many holes.

With the contour option I have to manually chain each hole.

Try selecting points using circlemill and setting your roughing options to what you need.

Link to comment
Share on other sites

Crazy,

Thanks for the input, the whole rough pitch field in helical bore seems broken, it should allow angles.

That said I think I have to quit using the helix bore and start using contour with ramp. it has the angle field option.

The only advantage to helical bore is that it uses the point selection option which helps when selecting many holes.

With the contour option I have to manually chain each hole.

 

I think helix bore is great for roughing and finishing holes...a very reliable toolpath as it always does what I want it to. I can understand your frustrations about angle/pitch. I have got used to using the pitch now, and i'll roughly put in a pitch that I think would be appropriate, then look at the graphic and see how the helix looks, and if the spiral is too steep for the diameter, i'll decrease it and vice versa. This is for solid carbide tools, I usually will stay a bit below 3 degrees...more like 1.5.

  • Like 1
Link to comment
Share on other sites

I think helix bore is great for roughing and finishing holes...a very reliable toolpath as it always does what I want it to. I can understand your frustrations about angle/pitch. I have got used to using the pitch now, and i'll roughly put in a pitch that I think would be appropriate, then look at the graphic and see how the helix looks, and if the spiral is too steep for the diameter, i'll decrease it and vice versa. This is for solid carbide tools, I usually will stay a bit below 3 degrees...more like 1.5.

 

+1

This sounds like the way I usually go about it. Most of the time I end up around 2 degrees. If there's room to move I'll step up the feeds pretty good.

 

Like Crazy said, there's so many of factors involved that's it's hard to go with a one fit's all.

Link to comment
Share on other sites

I haven't tried helix bore. I use circle mill and love it.

 

For a hole 150% the endmill diameter or so I am usually around a 6 degree angle. But it depends on how much room the endmill has to move, how deep the hole is, the material, etc. The harder the material the shallower the angle. I slow the feed down on the entry, then get after it on the way around.

Link to comment
Share on other sites

Something to watch out for when using circle mill. If you use a different feed rates for semi finishing and finishing, then change a feed rate, it will ignore the new feedrate and post the old one regardless of what is in the operation parameters. turning roughing off, regenerating, then turn it back on, then regenerate the operation again and the feedrates should post correctly.

 

 

 

http://www.emastercam.com/board/index.php?showtopic=67109

Link to comment
Share on other sites

This is for solid carbide tools, I usually will stay a bit below 3 degrees...more like 1.5.

 

I have been playing with 1.5 to 3 degrees and it seems like the sweet spot. Its just to bad you can't input 3 degrees into the Helic bore operation, "Set it and forget it!", but instead I do the math. But I may have found a quicker way to get rough pitch,

Center of cutter diameter divided by 6 will give me roughly 3 degrees, as opposed to getting circumfrence and multiplying by 3 degrees.

 

.625-.375=.250

.250/6=.041

 

 

As far as feedrate, my coworker suggested using,

c/b diameter minus tool diameter divided by c/b diameter multplied by normal feedrate

 

5/8 diameter c/b, 3/8 endmill. normal feedrate would be lets say 12. IPM

 

.625-.375=.250

.250/.625=.4

 

12 x .4= 4.8

 

4.8 IPM adjusted feedrate

 

These may not be optimal, but I am looking for more consistency than anything, so operators will at least know what to expect.

Link to comment
Share on other sites
  • 5 years later...
On 5/24/2013 at 11:01 AM, chipman said:

 

I have been playing with 1.5 to 3 degrees and it seems like the sweet spot. Its just to bad you can't input 3 degrees into the Helic bore operation, "Set it and forget it!", but instead I do the math. But I may have found a quicker way to get rough pitch,

Center of cutter diameter divided by 6 will give me roughly 3 degrees, as opposed to getting circumfrence and multiplying by 3 degrees.

 

.625-.375=.250

.250/6=.041

 

 

As far as feedrate, my coworker suggested using,

c/b diameter minus tool diameter divided by c/b diameter multplied by normal feedrate

 

5/8 diameter c/b, 3/8 endmill. normal feedrate would be lets say 12. IPM

 

.625-.375=.250

.250/.625=.4

 

12 x .4= 4.8

 

4.8 IPM adjusted feedrate

 

These may not be optimal, but I am looking for more consistency than anything, so operators will at least know what to expect.

hey just wondering if you meant .625-.3125  not .375. unless i read your comment wrong.

Link to comment
Share on other sites
1 hour ago, w_canas said:

hey just wondering if you meant .625-.3125  not .375. unless i read your comment wrong.

Quote

c/b diameter minus tool diameter divided by c/b diameter multplied by normal feedrate

Looks correct to me he said 5/8 Counter Bore using a 3/8 endmill. Do you have a specific question you need help with?

Link to comment
Share on other sites
  • 4 weeks later...
On 12/11/2018 at 7:14 PM, 5th Axis CGI said:

Looks correct to me he said 5/8 Counter Bore using a 3/8 endmill. Do you have a specific question you need help with?

I completely missed the c/b  and also misinterpreted the answer, i was thinking of something at the time, my bad.

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...