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:

Building High Feed Mills


JB7280
 Share

Recommended Posts

What tool type do you guys use when you build an indexable high feed mill?  I tried using the step file from Ingersoll's website, and applying it in a High Feed Mill, but none of the numbers are correct. 

https://www.ingersoll-imc.com/product/2906973

 

1341464830_Screenshot2022-08-29141819.thumb.jpg.c10cfed1a224e2ae5273f25c1c03dcc2.jpg

Link to comment
Share on other sites
Just now, crazy^millman said:

Bull endmill with the recommend radius. Sorry I am still not 100% convinced defining a highfeed cutter is the best process in Mastercam.

So, how does that work Ron?  They give a a recommended program rad of .094", but that would put my actual diamter at .812" when ingersoll claims it to be .594.

 

I initially had the same thought, however it seems like that would leave unexpected islands and pyramids?  If that method works well though, I'll continue defining them as bull endmills, as it's a whole lot simpler.  

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

So, how does that work Ron?  They give a a recommended program rad of .094", but that would put my actual diamter at .812" when ingersoll claims it to be .594.

 

I initially had the same thought, however it seems like that would leave unexpected islands and pyramids?  If that method works well though, I'll continue defining them as bull endmills, as it's a whole lot simpler.  

It is a 1.000 diameter bull endmill with a .094 Radius. You don't need to define the smaller diameter on a bull endmill.

Link to comment
Share on other sites
11 minutes ago, crazy^millman said:

It is a 1.000 diameter bull endmill with a .094 Radius. You don't need to define the smaller diameter on a bull endmill.

I'm missing something.  The green wireframe is a 1" bull endmill with .094rads, and the solid is the step file from Ingersoll.  Wont the areas in between be missed material?  Or is the step geometry wrong, perhaps?

 

1530731543_Screenshot2022-08-29143744.thumb.jpg.59a02768af1a56175083054f044b24de.jpg

Link to comment
Share on other sites

I have used highfeed cutters for almost 20 years and I have always defined them as bull endmills. This process has always worked. Why does it work I did a complete math breakdown of this many years ago and realized yes it leaving a little extra material when defining it this way verses the High Feed way, but when you see major performance hits in some areas of Mastercam using Highfeed Cutters for tool definitions I will stick with the KISS method here.

  • Thanks 2
  • Like 1
Link to comment
Share on other sites
37 minutes ago, crazy^millman said:

I have used highfeed cutters for almost 20 years and I have always defined them as bull endmills. This process has always worked. Why does it work I did a complete math breakdown of this many years ago and realized yes it leaving a little extra material when defining it this way verses the High Feed way, but when you see major performance hits in some areas of Mastercam using Highfeed Cutters for tool definitions I will stick with the KISS method here.

Sounds good.  Thanks Ron.  I'm just always worried about hitting one of those little ridges/peaks and going above the radius of the cutter.  Probably overthinking it though.  

Link to comment
Share on other sites

I've been using the High Feed tool and the manufacturer's step models for a couple of years now with no issues

I like doing this because you get accurate stock when you save an STL file out of a Verify session.

In the early days I had trouble with inserts getting crushed because the toolpaths were leaving cusps 

the tool was smashing into them during back feed moves .  That problem seems to be solved now.

In the example I've attached, I built a tool from an Ingersoll step file, then saved the geometry to a level

and edited it a little 

Notice in my example that I've lied in the Cutting length setting..

If I set it correctly the walls in a Verify session look like they've been cut with a .08R button cutter.

The resulting stl file was an unusable 120meg mess.

After tweaking the defining geometry and setting the Cutting Length to .300 my Verify STL's have nice clean walls

and yielded an 18 meg stl instead of a very messy 120 meg file

4in Ingersoll Hi Feed.jpg

  • Thanks 1
  • Like 4
Link to comment
Share on other sites
24 minutes ago, gcode said:

I've been using the High Feed tool and the manufacturer's stl files for a couple of years now with no issues

I like doing this because you get accurate stock when you save an STL file out of a Verify session.

In the early days I had trouble with inserts getting crushed because the toolpaths were leaving cusps 

the tool was smashing into them during back feed moves .  That problem seems to be solved now.

In the example I've attached, I built a tool from an Ingersoll step file, then saved the geometry to a level

and edited it a little 

Notice in my example that I've lied in the Cutting length setting..

If I set it correctly the walls in a Verify session look like they've been cut with a .08R button cutter.

The resulting stl file was an unusable 120meg mess.

After tweaking the defining geometry and setting the Cutting Length to .300 my Verify STL's have nice clean walls

and yielded an 18 meg stl instead of a very messy 12o meg file

4in Ingersoll Hi Feed.jpg

What was the purpose for the longer than reality cutting length?  What other editing did you do, aside from the cutting length?

 

I noticed you mentioned back feed.  Do you find that high feed mills do ok with dynamic toolpaths?  I've always leaned more towards contours, and area mill.  Toolpaths that make a more "uniform" toolpath.  Something about dynamic toolpaths with a high-feed mill makes me feel un-easy.  But you guys have far more experience than me, so I'm open to other methods.  

Link to comment
Share on other sites

I made a tool using an Ingersol High Feed step file

I was cutting a profile with it, a 12 paddle star shape 115" across and 10" deep

With an .08R corner radius and an .08" step down the walls of the verify stl were very ragged and nasty.

The stl file saved out at 120 meg. Making a stock model from it took forever and yielded poor results

so

I saved the tool geometry to a level, edited the geometry to create a fake .300" flute length.

Everything else matches the original stp file.

The results were clean wall, an 18 meg stl file and a very nice stock model.

The bottom of the tool produces an accurate representation of the stock and the fake

.300 flute leaves a nice clean wall.

I do use high feed in dynamic optipath with no problems

You need to use the bottom diameter of the tool to figure your radial stepover 

or you'll leave cusps behind that may cause trouble

 

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
I noticed you mentioned back feed.  Do you find that high feed mills do ok with dynamic toolpaths?  I've always leaned more towards contours, and area mill.  Toolpaths that make a more "uniform" toolpath.  Something about dynamic toolpaths with a high-feed mill makes me feel un-easy.  But you guys have far more experience than me, so I'm open to other methods.  

95% I use dynamic toolpaths with high-feed mill, so far it always worked!

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

As Gcode mentioned above, I cheated a little with cut length but the rest of the tool geometry is straight from STL.

I have used this with good effect in both dynamic and 'straight line' programming.

what I have come across is that the tool does not like machining over pre-drilled holes.

 

hi-feed.png

Link to comment
Share on other sites
9 hours ago, gcode said:

I made a tool using an Ingersol High Feed step file

I was cutting a profile with it, a 12 paddle star shape 115" across and 10" deep

With an .08R corner radius and an .08" step down the walls of the verify stl were very ragged and nasty.

The stl file saved out at 120 meg. Making a stock model from it took forever and yielded poor results

so

I saved the tool geometry to a level, edited the geometry to create a fake .300" flute length.

Everything else matches the original stp file.

The results were clean wall, an 18 meg stl file and a very nice stock model.

The bottom of the tool produces an accurate representation of the stock and the fake

.300 flute leaves a nice clean wall.

I do use high feed in dynamic optipath with no problems

You need to use the bottom diameter of the tool to figure your radial stepover 

or you'll leave cusps behind that may cause trouble

 

I think I get it.  So the purpose of that false flute length was to clean up the stl.  nothing to do with the actual real life part.  

 

The bottom of the tool issue is kind of why dynamic paths worried me with a feed mill.  So do you just try to use slightly less stepover than the bottom diameter?

 

Is there a chance you could post a file with one of your optirough feed mill toolpaths?  If not, it's cool, I'm just always curious to see other programmers' settings and methods.  

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

The bottom of the tool issue is kind of why dynamic paths worried me with a feed mill.  So do you just try to use slightly less stepover than the bottom diameter?

The tool mfg will provide adoc & rdoc numbers...I generally use Mitsubishi but their recomendations have usually been pretty good...I can't imagine Ingersol would be different in their suggestions

  • Thanks 1
Link to comment
Share on other sites
13 hours ago, gcode said:

I've been using the High Feed tool and the manufacturer's stl files for a couple of years now with no issues

I like doing this because you get accurate stock when you save an STL file out of a Verify session.

In the early days I had trouble with inserts getting crushed because the toolpaths were leaving cusps 

the tool was smashing into them during back feed moves .  That problem seems to be solved now.

In the example I've attached, I built a tool from an Ingersoll step file, then saved the geometry to a level

and edited it a little 

Notice in my example that I've lied in the Cutting length setting..

If I set it correctly the walls in a Verify session look like they've been cut with a .08R button cutter.

The resulting stl file was an unusable 120meg mess.

After tweaking the defining geometry and setting the Cutting Length to .300 my Verify STL's have nice clean walls

and yielded an 18 meg stl instead of a very messy 12o meg file

4in Ingersoll Hi Feed.jpg

Thank you for sharing that and letting everyone know how much better it is working. I will have to rethink my processes when I have another project requiring a highfeed cutter.

  • Like 1
Link to comment
Share on other sites
16 minutes ago, crazy^millman said:

Thank you for sharing that and letting everyone know how much better it is working. I will have to rethink my processes when I have another project requiring a highfeed cutter.

Ron, to your method, it seems that the "recommended programming radius" effectively leaves little enough material that it is small enough to not have an effect.  I'm sure you understand this already, but this diagram helped make a little more sense of it to me. 

1360963386_Screenshot2022-08-30073645.thumb.jpg.32cc494974c5c9b72f0bc280cbd053f5.jpg

  • Like 1
Link to comment
Share on other sites
2 hours ago, JB7280 said:

I think I get it.  So the purpose of that false flute length was to clean up the stl.  nothing to do with the actual real life part.  

Correct.. the walls of the real life part look like crap because they are machined by an .08R stepping down .08"

but I don't care because there is still stock

Mastercam's stl file is a different story. The .300 cut length yields fake spring passes that leave a smooth clean dimensionally  correct STL file and a much more user friendly stock model

24 minutes ago, JB7280 said:

Ron, to your method, it seems that the "recommended programming radius" effectively leaves little enough material that it is small enough to not have an effect.  I'm sure you understand this already, but this diagram helped make a little more sense of it to me. 

1360963386_Screenshot2022-08-30073645.thumb.jpg.32cc494974c5c9b72f0bc280cbd053f5.jpg

 

 

This is the safest way to program high feed cutters.

You will never gouge your part using this method. However, the stock you get in verify will not be accurate.

For small tools this probably doesn't matter.

For the Ø4 to 6" Ingersoll I'm using that remnant can be a tapered floor  .180" thick by .350 wide and needs to be present in your stock models

Link to comment
Share on other sites

I get them from the insert specs.

But

Some manufacturers have such complex insert geometry that it is impossible (and pointless) to model it.

Check out the Mitsubishi AJX line of high feeds for an example of this

 

 

 

Link to comment
Share on other sites

I have been using high feed mills for a long time as well. I do not like how mastercam handles some toolpaths with the highfeed tool geometry so I will define it as a bullmill occasionally for the dynamic or legacy toolpaths. The tool manufacturing models are usually not perfect 1:1 models either and I typically just use the dimensions they give on the websites to define my tools and I haven't had a problem defining them using this system (https://catalog.tungaloy.com/Item.aspx?cat=6993972&fnum=1297&mapp=ML&GFSTYP=I&srch=1).

Link to comment
Share on other sites

In the past, I programmed them as a bull mill with the tool manufacturer's geometry for accurate stock model.  But I had problems with cusps that would interfere with my Dynamic/Optirough operations.  It was a hit or miss situation and I had to verify the toolpath after any parameter change to make sure that I wasn't leaving cusps.

I thought  that I would try the High Feed tool definition again and see what I can get.

I brought in a High feed mill model and let Mastercam try to define the tool automatically.  This is what I got

2022-09-07_1-20-56.png.c417054ccce399cb178d34b9ca5b49e7.png

Then I started playing with the parameters and was able to get a much closer profile.  I matched the manufaturer's tip diameter, extended the length and was able to add the relief taper angle.  This is what I ended up with:

2022-09-07_1-32-04.png.437b4cba89b777ae9b24487b592a0c12.png

So far, after trying different stepovers and other parameters in Optirough, I have not gotten any leftover cusps.

 

Thanks Tom, et al for this thread

  • Like 5
Link to comment
Share on other sites
  • 2 weeks later...

I ran into a most unexpected result today when using a tool defined as a high feed mill.

I am using Mcam 2022 for this part.

Sorry, I can't share this file.

After defining the tool in the thread above, I used it in a very large part and this is the optirough toolpath that was generated:

519641642_highfeedmillcut.png.c96b41ab65cfed4e393820b85a8783b2.png

 

I changed the cutter to a bull nose with embedded geometry from the manufacturer's STEP file and then made NO other changes and regenerated the operation and this is what I got and what I was expecting:

787515011_bullnosemillcut.png.1b4ddcaae14598de4819ffba8e81501a.png

I went back and double checked everything and there is definatly something going on with Mastercam using some of the information from the high feed definition to keep it from stepping down a vertical wall and ruining the outside edge of the insert.

 

BUT it is not consistent.  I generated some other toolpaths with the high feed cutter definition and it worked as I expected.

 

The cutter is a Sandvik 2.0 dia. MH20 cutter which they are calling a "High-feed pocketing"  cutter and it works well for that application.  I ran a test in 4140 at Vc=625, Fz=.031, Ae=1.3, and Ap=.045.  after 27 minutes in cut, I couldn't see any wear on the insert and the outside corner wasn't blown out.

2112046662_mh20demopart.thumb.png.3028df181d7be82dc3acd9a6718afcbd.png

After 27 minutes:

insert.png.d3adadfd603c8c0e7d58454ed622c337.png

 

So: I am back to defining high-feed cutters and bull nose and will deal with the cusp problem because I need to be able to step down veritcal walls.

 

I am going to reach out to Mastercam and see if they can offer some insight to when this happens and if there is a way to turn it off.

 

 

 

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...