How to define a custom cutter -- Harvey 26802 Double Angle cutter

[Finegrain]

Hi guys,

New here, .5 yrs MCAM Mill + 1.5 yrs MCAM Lathe user ...

I am going to be using a Harvey 26802 double angle cutter to deburr the backside of a 5mm hole, plus the frontside of another 5mm hole on the same axis but deeper. First thing I need to do (I think) is define the tool in my tool library -- what are the basics for that -- create a model of the tool and point the tool library at the model? How should the model axes go? Tool axis centered on Z I assume, then Z = zero at the tip of the tool?

After I have the tool defined, how can I tell MCAM to use the "other" side of the double angle cutter to do the work for the backside deburring? In the chamfering dialog, it seems that the only option is to specify the tip offset, not the "other side" offset.

Sorry if these are goofy ways to describe the scenario

Regards.

Mike

[Guest]

Easy, you tell the user(you) to calculate the numbers to use the other side of the cutter and use those numbers.

There is not an "automagic" way to do it

 

 

 

[So not a Guru]

9 hours ago, Finegrain said:

Hi guys,

New here, .5 yrs MCAM Mill + 1.5 yrs MCAM Lathe user ...

I am going to be using a Harvey 26802 double angle cutter to deburr the backside of a 5mm hole, plus the frontside of another 5mm hole on the same axis but deeper. First thing I need to do (I think) is define the tool in my tool library -- what are the basics for that -- create a model of the tool and point the tool library at the model? How should the model axes go? Tool axis centered on Z I assume, then Z = zero at the tip of the tool?

After I have the tool defined, how can I tell MCAM to use the "other" side of the double angle cutter to do the work for the backside deburring? In the chamfering dialog, it seems that the only option is to specify the tip offset, not the "other side" offset.

Sorry if these are goofy ways to describe the scenario

Regards.

Mike

I use the circle mill path, with a combination of the incremental depth linking setting and the stock to leave on walls & floors.

In your case, if I wanted a .01" chamfer on the bottom of the hole. I'd select the arc, set the stock to leave on walls to -3/64"( the radial center of this cutter's "V"), the stock to leave on floors to -9/128+.01 ( the axial center of this cutter's "V", plus my chamfer).

Then I would make all of my linking depth incremental at 0.0".

Be sure to set your transitions to lead in/out, start at center.

 

[Rstewart]

You'll need to draw the tool 2D geometry if you want to see what your doing in verify.  You just draw the radial tool profile with the bottom of the cutter at X0 Y0 in the positive quadrant from top view.

This has been explained several times, just do a search on this forum.

[Guest]

This is how a custom tool should look drawn in mcam

 

[Orvie]

Attached is your tool & the DXF required to link it in Tool Manager.

26802.dxf

26802.tooldb

[The Cathedral]

Harvey has .dxf for all their tools on their website so you don't have to draw them from scratch, but you do have to fiddle with them to make them work with Mastercams requirements.

As for toolpathing, everybody is correct in that there is no "easy" way to do it since the back chamfering functionality does not exist in Mcam. I do this all the time and the best way to do it is with a calculator and verifying the toolpath with simulator.

 

[Tim Johnson]

I just click the entity that I'm going to chamfer. For a .010 chamfer I set the leave stock allowance to X-.03 and Z- tool bottom to cutting point distance  - .02.

[HEAVY METAL]

Yes, I just downloaded a tool  profile yesterday from Harvey .    DXF   --------  very handy  make it easy to create  a custom tool .

[nickbe10]

We use Harvey tools a lot for this sort of thing. Keep an eye out  when you import .DXF files from Harvey for extra hidden geometry.

I don't know if it is our computer system or something else but I always get one tool profile on MC origin and another hidden profile off the origin.

I just always check for hidden geometry and get rid of it to avoid confusion

Nick Eaton

CNC programmer

Primus

[Guest]

2 hours ago, nickbe10 said:

We use Harvey tools a lot for this sort of thing. Keep an eye out  when you import .DXF files from Harvey for extra hidden geometry.

I don't know if it is our computer system or something else but I always get one tool profile on MC origin and another hidden profile off the origin.

I just always check for hidden geometry and get rid of it to avoid confusion

Nick Eaton

CNC programmer

Primus

I always just do it and delete the geometry that is  blanked after the first time I found....

Import the dxf, unblank geometry, select that and delete

[Joe6Pack]

I use these tools every day. They're easy to program.

The 26802 is a 3/16 dia and the center of the < > is .0465 from the tip.

Use any tool path you want; contour, circle mill, etc, geometry is on the theoretical sharp edge

For a top surface edge break, linking param depth is incremental 0.0, top of stock incremental 0.0, stock to leave on walls is -.01+-, stock to leave on floor is -.0415 (Z -.0465 to tool sharp edge plus Z .005.

for a back chamfer, change the floor "stock to leave" to the other side of the < > centerline; -.0515 (-.0465 -.005 = Z-.0515)

Essentially you are programming the sharp intersection of the tool to incremental Z 0.0 then shifting +- .005 for top or back chamfer. Once you have the sharp corner distance for each size, jot them down and stick on the wall.

 

[scooch8292]

I'm kind of having the same issue here. Trying to define a new slot mill cutter. There's nowhere to put in a neck diameter or length. I used the dxf file from Harvey for their tool #43562, cleaned it up, made sure all lines where connected, no overlapping entities, no hidden features and I get this (see below). It would be nice if we could enter a neck length and diameter for slot mills.  Right now our shank diameters, are designed  using the neck diameters, for all our slot mills. Any ideas on how to get around this properly?

[Orvie]

You can do this using and endmill tool definition, but you will not be able to put a radius on the top edge.

 

https://www.dropbox.com/sh/smr3vo9js7u9a3x/AACA7vVrqZNCACCAvIa3auONa?dl=0

[scooch8292]

Yeah, been there done that and wound up ordering duplicate tools because it did not show up in the slot mill selection when filtered. True story.