Building High Feed Mills

[Bill Craven]

Ah...

Thanks Tom,  I will give that a try.

[Bill Craven]

Okay,  I tried that.  I made it .25   Not much change.  Then I made it .45 for the LOC.  That made it better but it is still way off what 

The cutter path is now not even close to model.

 

It should look like this:

 

 

[gcode]

Can you share the tool

[Bill Craven]

high-feed.zip

Yes sir,

it is attached.  2022

[gcode]

I think you need to break that up

You've got the tool and a Capto arbor mated into one step file defined as a tool

If you select Render Mastercam Tool, you'll see what is actually being used to compute the tool paths

The tapered adapter can't be accurately described by the fields in the tool definition

(at least that's my understanding of all this)

Try defining the tool by itself, and then define the Holder with a separate STL file  

[crazy^millman]

1 hour ago, gcode said:

I think you need to break that up

You've got the tool and a Capto arbor mated into one step file defined as a tool

If you select Render Mastercam Tool, you'll see what is actually being used to compute the tool paths

The tapered adapter can't be accurately described by the fields is the tool definition

(at least that's my understanding of all this)

Try defining the tool by itself, and then define the Holder with a separate STL file  

I am with Gcode on this. I never put any of the shanks into my tool definition. I always make them part of the holder definition.

[gcode]

You have to be real careful with Sandvik tool models

The step file for this tool is not right. The white portion of the model which represents the insert is actually surfaces

and does not come in when you create a tool with the step file.

That's what Mastercam's tool manager says the tool diameter is 1.93 instead of 2"

[Bill Craven]

First off, I want to say how much I appreciate this forum.  Thank you all very much.

I tried several different things and will list them below.

I changed the shank diameter to 1.7 from 1.997 and the toolpath regenerated the way that I wanted it to.  this is the quickest solution, but not necessarily the best.

I built the tool definition just using the tool and inserts and then brought in the holder from a STEP file of the holder and extension.  I can see where this will probably give better collision detection.  but now my tool holder library just became pretty much obsolete and assembling holders and extensions will be more time consuming and difficult keeping track of all of the variations.  I was concerned that my setup sheets might not show the correct gauge length, but that worked fine.

 

I am aware of the incorrect STEP models.  You get better results if you save the detailed models.  For the detailed model, I ended up with a 1.997 diameter cutter.  Better but not perfect.  I don't know what their tolerance is for that cutter 

 

I also built up a tool definition based upon a wireframe.  The advantage to doing that is that I can simulate the undercut on the face.  I always generate a wireframe tool when doing turn milling.  I always make sure to break the link to the level that the geometry is on so that I can save that tool to a library and use it in other programs.  I used the holder extension combo for the holder

 

[gcode]

Is this tool giving you good results

[#Rekd™]

Tons of great information in this thread, should be pinned for a while.

 

 

[Bill Craven]

2 hours ago, gcode said:

Is this tool giving you good results?

Yes,  It has amazed me.  In theory, I am removing around 12 cubic inches per minute (Because it is an Optirough dynamic path, I am probably only getting 50-60% of that due to slices in corners etc.  Still very respectable.)

2.0 diameter cutter.  Material=4140 steel.  SFM=625, ftp=.031, feedrate=196 ipm, depth of cut=.045, stepover=1.3, hp=11, no coolant.  Some vertical walls.  

After 27 minutes I couldn't tell which edge had been used.    The only way I could tell was that there was a little discoloration on the chip-breaker.  I expect that I should be able to go for an hour before indexing the inserts.  

[gcode]

I was asking if the latest version of the high feed  tool was generating a good toolpath in Mastercam,

or are you still running the bull endmill definition?

[Bill Craven]

2 hours ago, gcode said:

I was asking if the latest version of the high feed  tool was generating a good toolpath in Mastercam,

or are you still running the bull endmill definition?

Sorry, I misunderstood. 

 

I am running it as a high feed, but haven't actually cut anything yet. 

When I have time, I still need to run some more tests to verify that my issues with cusps are better.

I am also trying to use the create tool assembly (which I have not used before) so that I can more easily keep the tool separate instead of building a STEP file with the cutter and extensions and adapters.  I like the tool assembly concept but it causes problems with my Active Reports setup sheets because it lists the holder as the adapter that is just above the tool and then says "Composite"    I want my setup sheet tool list to have all of the parts of the tools listed so that the setup person will have all of the tool part numbers for setup.

[gcode]

35 minutes ago, Bill Craven said:

  I want my setup sheet tool list to have all of the parts of the tools listed so that the setup person will have all of the tool part numbers for setup.

agreed

For mission critical tool lists with Capto stacks I make a SolidWorks assembly of each tool  and use that to create a tool sketch

It's a ton of work.

an automated solution would be nice

I looked into some tool management software packages, but the prices were breathtaking

and I could not get approval to move forward. 

 

[crazy^millman]

33 minutes ago, Bill Craven said:

Sorry, I misunderstood. 

 

I am running it as a high feed, but haven't actually cut anything yet. 

When I have time, I still need to run some more tests to verify that my issues with cusps are better.

I am also trying to use the create tool assembly (which I have not used before) so that I can more easily keep the tool separate instead of building a STEP file with the cutter and extensions and adapters.  I like the tool assembly concept but it causes problems with my Active Reports setup sheets because it lists the holder as the adapter that is just above the tool and then says "Composite"    I want my setup sheet tool list to have all of the parts of the tools listed so that the setup person will have all of the tool part numbers for setup.

Bill the inherit problem with assemblies is there not a process for externally supporting them. Yes it sucks having to build models for your assemblies to then make them holders, but I have found making them this way gives the ability to control their naming. By using the assembly process in Mastercam you have some major disconnects. You cannot mate them like you can in Lathe. 3D lathe for handing 3D tools is the way Mill Should work, but in it current state it is servery lacking in functionality and capability. That said I still build all my 3D lathe tools as models and not as components.

 

[Bill Craven]

4 hours ago, gcode said:

For mission critical tool lists with Capto stacks I make a SolidWorks assembly of each tool  and use that to create a tool sketch

It's a ton of work.

Yes, I believe that is the very definition of a ton of work.  And then even more work to bring them into Vericut...

 

Okay, So I ran some more tests with the high-feed tool definition and didn't have any cusps.  (I may be on the 'Cusp of success' with this.  Now is the time for a collective groan)

My tool build strategy going forward will be to use the tool and inserts STEP model define the tool and give it the proper names.  Then build a solid model for the holder and adapters and name the holder with the proper names.  

That looks like it will work well.  I'd post a picture, but I don't have any kbs left for embedding 

[crazy^millman]

59 minutes ago, Bill Craven said:

Yes, I believe that is the very definition of a ton of work.  And then even more work to bring them into Vericut...

 

 

Nope use the Interface and once built it carries all the way through into Vericut. 3D lathe tools are supported also.