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:

High feed face mill


jean
 Share

Recommended Posts

That is not a bad way to do it. Another way that is better in Mastercam using that tool I cannot think of one. I would try dynamic with a solid tool full flute and see if it is faster thought I doubt it would be. At 1 minute 30 seconds of a backplot time that is impressive. Anyone who say they can do it faster are more than welcome to step up and teach us both. Using the same SFM as the High Feed with Dynamic and 25% step over I can get 1 minute 35 seconds with the .004 per tooth feed rate defined on the 1" Endmill. I kick it up to .006 per tooth I get 1 minute 4 seconds time again with 25% step over. The High Feed cutter process you are using without seeing the setup, rigidity of the machine and other things it would seem is probably still the best way.

Link to comment
Share on other sites

Here is my take on it. Seemed to be just a bit of recutting, by tracing the whole contour. So I just built my own wireframe, after measuring the width across those faces.

I did some digging on that tool definition, and couldn't find those part numbers on Kennametal's website. Are they perhaps old part numbers?

Closest I found (based on 7-flutes, and 2.5" diameter) was this:

SAP Material Number    6025275
ANSI Catalog Number    7792VXD12-A063Z7R
[D1MAX] Maximum Cutting Diameter    2.480
[D] Adapter / Shank / Bore Diameter    .8666
[D1] Effective Cutting Diameter    1.764
[D6] Hub Diameter    1.771
[L] Overall Length    1.574
[AP1MAX] 1st Maximum Cutting Depth    .0984
[Z] Number of Flutes    7

Based on their recommended starting feeds, at 40-100% Stepover, and .098" stepdown (2.5mm per pass), they are recommending between 0.44mm and 0.49mm per tooth. That would be about 0.017"-0.020" per tooth, so about 250 IPM for that 7-flute feed mill.

Check out the path, and results...

 

Feed mill_custom-contour.mcam

  • Like 2
Link to comment
Share on other sites
14 hours ago, Colin Gilchrist said:

Here is my take on it. Seemed to be just a bit of recutting, by tracing the whole contour. So I just built my own wireframe, after measuring the width across those faces.

I did some digging on that tool definition, and couldn't find those part numbers on Kennametal's website. Are they perhaps old part numbers?

Closest I found (based on 7-flutes, and 2.5" diameter) was this:

SAP Material Number    6025275
ANSI Catalog Number    7792VXD12-A063Z7R
[D1MAX] Maximum Cutting Diameter    2.480
[D] Adapter / Shank / Bore Diameter    .8666
[D1] Effective Cutting Diameter    1.764
[D6] Hub Diameter    1.771
[L] Overall Length    1.574
[AP1MAX] 1st Maximum Cutting Depth    .0984
[Z] Number of Flutes    7

Based on their recommended starting feeds, at 40-100% Stepover, and .098" stepdown (2.5mm per pass), they are recommending between 0.44mm and 0.49mm per tooth. That would be about 0.017"-0.020" per tooth, so about 250 IPM for that 7-flute feed mill.

Check out the path, and results...

 

Feed mill_custom-contour.mcam 5.82 MB · 3 downloads

With these parameters, and custom built wireframe geometry (and modified based on backplot/verify results), I'm showing 43 seconds with this 2.5" (63mm) High-Feed Face Mill.

I'm using 0.095" Step Down, and 250 IPM. I don't know the material, but at the programmed 2,089 RPM, we're showing 1375 SFM.

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

With these parameters, and custom built wireframe geometry (and modified based on backplot/verify results), I'm showing 43 seconds with this 2.5" (63mm) High-Feed Face Mill.

I'm using 0.095" Step Down, and 250 IPM. I don't know the material, but at the programmed 2,089 RPM, we're showing 1375 SFM.

I'm sorry, Ductile Iron.

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

Here is my take on it. Seemed to be just a bit of recutting, by tracing the whole contour. So I just built my own wireframe, after measuring the width across those faces.

I did some digging on that tool definition, and couldn't find those part numbers on Kennametal's website. Are they perhaps old part numbers?

Closest I found (based on 7-flutes, and 2.5" diameter) was this:

SAP Material Number    6025275
ANSI Catalog Number    7792VXD12-A063Z7R
[D1MAX] Maximum Cutting Diameter    2.480
[D] Adapter / Shank / Bore Diameter    .8666
[D1] Effective Cutting Diameter    1.764
[D6] Hub Diameter    1.771
[L] Overall Length    1.574
[AP1MAX] 1st Maximum Cutting Depth    .0984
[Z] Number of Flutes    7

Based on their recommended starting feeds, at 40-100% Stepover, and .098" stepdown (2.5mm per pass), they are recommending between 0.44mm and 0.49mm per tooth. That would be about 0.017"-0.020" per tooth, so about 250 IPM for that 7-flute feed mill.

Check out the path, and results...

 

Feed mill_custom-contour.mcam 5.82 MB · 5 downloads

I'm sorry you are correct.

Feed mill : 6025583

Insert: 6033257

Kennametal high feed.png

Link to comment
Share on other sites

https://www.kennametal.com/us/en/products/p.xdpw12-d-precision-pressed-with-reinforced-geometry-first-choice-for-hardened-materials-and-cast-iron.6033257.html#tad

With that EDP# for the insert, and based on the insert geometry, I found the following Feed Table (in metric values), at the bottom of the post.

With the recommendations you posted, the recommended Feed per Tooth you gave (at 0.01186" per tooth), is only 0.3mm per tooth.

More importantly, look at the range of feed values. On the low end, we have 0.22mm per tooth, on the high end, 0.82mm per tooth.

I think with those numbers you listed (173 ipm), that is running on the very conservative side of the tool. (low end of the feed values). Nothing "wrong" with that per se, but you're leaving some performance on the table for sure.

You could easily do between 250-350 IPM, using those inserts and that mill body, in Cast Iron, with 40-100% stepover.

Something to note about the drawing you posted: the calculations are being made based on the "diameter of the flat", not the diameter at the periphery of the tool. I'm not sure how that plays into their calculations of feed-per-tooth, but I thought it worth mentioning...

Kennametal Feed Mill Insert Feeds.PNG

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

Here is my take on it. Seemed to be just a bit of recutting, by tracing the whole contour. So I just built my own wireframe, after measuring the width across those faces.

I did some digging on that tool definition, and couldn't find those part numbers on Kennametal's website. Are they perhaps old part numbers?

Closest I found (based on 7-flutes, and 2.5" diameter) was this:

SAP Material Number    6025275
ANSI Catalog Number    7792VXD12-A063Z7R
[D1MAX] Maximum Cutting Diameter    2.480
[D] Adapter / Shank / Bore Diameter    .8666
[D1] Effective Cutting Diameter    1.764
[D6] Hub Diameter    1.771
[L] Overall Length    1.574
[AP1MAX] 1st Maximum Cutting Depth    .0984
[Z] Number of Flutes    7

Based on their recommended starting feeds, at 40-100% Stepover, and .098" stepdown (2.5mm per pass), they are recommending between 0.44mm and 0.49mm per tooth. That would be about 0.017"-0.020" per tooth, so about 250 IPM for that 7-flute feed mill.

Check out the path, and results...

 

Feed mill_custom-contour.mcam 5.82 MB · 5 downloads

Thanks for this different approach, I like it. That's what I was looking for a different insight. 

Much appreciated.

  • Thanks 1
  • Like 1
Link to comment
Share on other sites

I had a really nice response to this written up. Opened the catalog to look something up and lost it.  Dummy me

Long story short. Seeing as this is my day job...

  If indeed you are running that long tunable adapter.  You will likely need to drop DOC down to .020-.040".  Unless it is 65-45-12 DI and is soft as butter, do not run those at 1200 sfm, treat it like one might steel or use K3 material group numbers, run those D KCK15 inserts at 700-800 SFM, and start around .040" on the feed.  If those don't hold up due to chipping or built up edge, switch to KCPK30 in the GP chip breaker, and run 550 SFM, and .040" on the feed.  Same light depth.  If it is stable, feel free to walk the depth up until it isn't and back it off a bit to regain stability.

Oh and ramping is going to more than double the radial load, so avoid it if you can in this case.  If you can't avoid it due to fixture constraints, you can't...

FYI for the group 7792 inserts should not be run at over 80% of max ap1 listed for it's IC size. When shouldering it can't be avoided at the wall, but it can handle it there due to chip thinning, if you run that deep you will likely blow the corners off the insert at any feed over .015 ipt.  Lower depths of cut at higher feedrates are almost always more productive.

  • Like 2
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...