No tool offset (ie cut along the tool's 'centre' point?)

[HankMcSpank]

Hi There,

I'm just creating simple 2D stuff, but I would like to take the edge off the perimeter (essentially chamfer) on a piece I'm cutting out.

What I'm wanting to do is use a ball nose endmill & run it around this said perimeter (prior to running the standard full through the material cut on the same perimeter), but without any compensation ...in other words I just want the cutting tool to run around the actual perimeter line as opposed to a small offest (which Mastercam typically allows/compensates for the cutter's radius when forming the toolpath)

A seemingly simple requirement, but I can't establish a way to do this (when I select 'compensation 'off' in paramaters, I don't see any toolpath afterwards!) - please give me a pointer!

[Superman]

Originally Posted by HankMcSpank A seemingly simple requirement, but I can't establish a way to do this (when I select 'compensation 'off' in paramaters, I don't see any toolpath afterwards!) - please give me a pointer!

Hi Hank
Comp OFF tells mastercam to not to insert G41/42 into the program, if you also have an XY offset of zero, the toolpath will on top of the selected contour, backplot it to actually see the path or view at a slight angle

Using a ballnose is a little more awkward and you have to fudge the numbers to get what you want, mastercam uses the tool dia for the comps when using a flat, bull, or ballnose cutter, the other forms use the base dia ( point dia) for the calculations ( ie facemill, tapermill, chamfermill ). You may have to draw a semicircle and work out depths and offsets

Try using for a 10mm ball ( approx values only )
top of stock=0 abs, Depth=0 abs
Comps OFF, XY offset= 3, Zdepth= -1
or
comps WEAR, XY offset= -2, Zdepth= -1

Either of these should put the ball on the profile, adjust depth or offset to cut deeper

[HankMcSpank]

Originally Posted by Superman Hi Hank Comp OFF tells mastercam to not to insert G41/42 into the program, if you also have an XY offset of zero, the toolpath will on top of the selected contour, backplot it to actually see the path or view at a slight angle Using a ballnose is a little more awkward and you have to fudge the numbers to get what you want, mastercam uses the tool dia for the comps when using a flat, bull, or ballnose cutter, the other forms use the base dia ( point dia) for the calculations ( ie facemill, tapermill, chamfermill ). You may have to draw a semicircle and work out depths and offsets Try using for a 10mm ball ( approx values only ) top of stock=0 abs, Depth=0 abs Comps OFF, XY offset= 3, Zdepth= -1 or comps WEAR, XY offset= -2, Zdepth= -1 Either of these should put the ball on the profile, adjust depth or offset to cut deeper

Thank you Superman,

In the light of your confirmation that 'compensation' should be set to off...I went back for another look. Doh...yep, sure enough the tooolpath is there, but the toolpath colour (blue) is virtually obscured by the endpoint line colour (green)....I didn't see this the first time.

re your suggested values, firstly, I don't have a 10mm ball, I only have a 3mm ball (the acrylic I'm cutting is only 2.6mm thick, so a 3mm ball ought to be ok to just take the hard edge off the perimeter). To give you an idea, here's what I've made....

(it's my first attempt...so please don't criticize!)

I'm cutting the bits individually, top middle * bottom - I just want to take the harsh top edge off the top & bottom pieces)

The trouble is, the default values are sinking the ball into the edge (which figures) & I end up with a concave vibe...no matter what depth I use. I need an xy offset...which is what you've alluded to...but where do I put those offsets? (could you be 'newbie' specific please?!!)

Many thanks once again - a great help.

[Superman]

I'll scale it down from 10 to 3mm
use Pythagoras 3,4,5 triangle

Try for a 3mm ball ( approx values only )
top of stock=0 abs, Depth=0 abs
Comps OFF, XY offset= .9, Zdepth= -0.3
or
comps WEAR, XY offset= -0.6, Zdepth= -0.3

Either of these should put the ball on the profile, adjust depth or offset to cut deeper

Have you tried defining a chamfermill for creating chamfers ( really easy ) ?

2 examples
Spotting & Chamfering
http://www.iscar.com/Ecat/item.asp/a...604521/lang/EN
Chamfermill_base Ø = 1.5 , angle 45, shank Ø=10, flute L=4.25

Chamfering only
http://www.iscar.com/Ecat/item.asp/a...621404/lang/EN
Chamfermill_base Ø = 1.95 , angle 45, shank Ø=10, flute L=4

The critical size is the point Ø of the tool, would be better to make it bigger to stay off further.

When defining a Chamfer op on a 2D contour, select the contour you wish to chamfer, accept, select a chamfer tool, select operation type (2D chamf, ) in pull-down on parameter page, select the options push button beside it and set how big you want the chamfer, & how far you you want the end of tool to project past the bottom of chamfer.

We use as deburr defaults ( depth must be the top edge of the chamfer )
0.2mm chamfer size ( how much of the contour you want removed )
1.0mm tool project past ( zero makes the tool level with the bottom of the chamfer, 1mm allows a little more project so to use exactly 45° part of tool, note allow for the curvature formed by the web thickness of the "spotdrills" )

This will post a program with chamfering of the top face @ Z-zero, tool's actually cutting depth will be Z-1.2, where Z-1.0 would cut nothing off the part and leave a theorical sharp edge.

Just a comment in passing
The bigger the radius of the tool -- the flatter a cut will seem to be

Ø10mm would be good, my numbers would put the cutting point on the rad near 50°, where 0° is the bottom of the tool

[HankMcSpank]

Many thanks Superman...I had limited success using a ball end to chamfer! (not for want of you trying to help though!).

Today I managed to find/buy a 3.2mm shank rounding bit with a 2.5mm radius - perfect!

That said I'm getting somewhat unexpected results when I go for a toolpath 'verify'.

first here's the tool I bought...



& here's how I've created a new tool...



(not sure if I selected the right type when I created - it looked most like a rad mill from the Mastercam illustrations)

I'm getting a little confused with how to set the paramaters up now - how should I set the toolpath parameters up, so the whole of that cutter 2.5mm radius 'cuts' into the contour edge?

Basically, when I go for a verrify, if I set the depth to 0, then I see the rounded edges appear onscreen...but then in practise, when I zero my cutting tool on the workpiece, it just runs around the top of the countour without cutting down into it! I can workaround this by settingthe depth to 2.5mm, but then the verify shows the toolpath as going down 'past' the radius part of the cutter & cutting my part with the flat perpenduclar upper part of the tool.

it's be nice to have the verify match up with the practise...wheich must mean I've either set the library tool up wrong or not got the right parameters.

Puzzled.

Many thanks.

[Superman]

Hi Hank,

Your tool setup page looks good, the pilot diameter is critical as this is what Mastercam sets away from your contour
Tool tip zero point when gauging this tool for your machine is thru the R2.5 centre point ( note!! the spelling ).

In Mastercam, the contour parameters page
Feed plane=1.0 inc
Top of stock=top surface of the rad.
Depth= same as top of stock
Contour type=2D
Comp=Wear
Comp Dir=Left
Tip comp=tip
XY stock to leave = 0.1 ( programmed path is .1 off the actual finish line- allows a little bit of comp )
Z stock to leave = -2.5 ( puts your tooling gauge point this far below the actual contour
Lead in /out= as you prefer
Filter= create arcs in XY ( minimum )

Don't use multi passes or depths yet ( get the single pass to verify correctly 1st)

Steve

[HankMcSpank]

Hi Superman,

Thanks once again for taking the trouble to help me.

When I use those suggested settings, I don't see the rounded outer edge on my part (the outside edge is the contour I want the 'rounding' to happen on)...



if I change the depth setting to '0' I do see the rounded edge in verify...




but from recollection, that was was the setting where when I went for the actual cut on my machine, the tool tip only plunged the top of the stock (which is how I set the zero point) & didn't sink into it....it just moved all the way around the contour immediately above it!

Any ideas how I can be getting this disrepancy between verify & an actual cut?

[Superman]

On the contour parametrs page, Try changing "tip comp" to tip not centre ( 99.9% of the time, it should alway be "tip" ). This is where your main problem lays.


and check your chain in the geometry section, big green arrow pionts in the direction of cut, and the small arrow indicates the offset side
( big arrow should point CW, little arrow points to the left-the side the tool will run )

[HankMcSpank]

Hi Superman,

Ok...I tried that - I now get a curve in verify at least!

I'll let you knwo how I get on with the actual real life cut later today.

Be useful to know when 'centre' should be used vs 'tip' on the 'tip comp' parameter setting though?

[Superman]

Rob
One scenario where "centre" would be used is take a 1/2 pipe
and you wish to create a path over the arc of this pipe

If you look from the side, picture the path if you had the "Tip" and "Centre" programmed seperately
-Tip- would show a path starting below the centre-line, moving up to the crest of the arc and down the other side, mastercam would output this as point to point code. You could end up with 1000 lines of code for one pass.
-Centre- would show a path starting at the centre, and be 1/2 the tool away from the pipe and it would remain at this distance over the arc to the corresponding point on the other side, mastercam would output this in one line of code ( a 180° arc )

You have to picture that mastercam calculates the path to go thru this setting point on the tool, and you have to set it the same in the machine

A point to note, is if you use centre on one tool, it must be continued thru the entire program
You cannot mix the types on the same tool

I'm glad that you got verify to show the path correctly
( wait until you do 4 or 5 axis stuff, even mill/turn, then you can get angry if it don't work )

Steve

[Andre' B]

Originally Posted by Superman A point to note, is if you use centre on one tool, it must be continued thru the entire program You cannot mix the types on the same tool

As long as you use different offset numbers it should work fine.

[cadcam]

Review these picture and see if this helps.