Cutter compensation..

[driftmaster]

Hello.
New here at the forums, i will probably find the answer in some thread but i'm too lazy right now =)

I'm using Mastercam 9.0 for my "small" home projects, with a mill using fanuc (don't remember what version) but anyways, i'm having problems when using cutter compensation (wear)..it generates too short path (imo), If using for example G41 it reads it and moves only 1mm in X and nothing in Y, i would like to make that moting a bit longer, but how?

I'm not very familiar with the program but i have tried everyhing i can think of without any success..

Any help would be great!
And sorry for my bad english =)

[timlkallam]

Insted of wear use control it will generate a toolpath a least the radius of the cutter.

[Superman]

For V9.0, you have 2 options

1/- extend your geometry
2/- use "Lead in/out" , this will add additional movement to the start and endpoints of your contours , the arc is the entity the connects to your geometry , the line is the extension onto the arc along which the cutter comp. is taken up, ( or if at the end, cancelled )

On many machines, cutter comp is taken up or cancelled on a line only
-if you use "Wear" , then the compensation value in the control should be 0(zero) , lead in / out ( lines & arcs ) can be zero or +ive. ( you are programming the tool centreline)
-if you use "Control" , then the compensation value in the control should be the tool radius , lead in / out ( lines & arcs ) can be zero or greater than the tool radius.( you are programming to the part contour )

If you can get V9.1 or .2 - go for it , it has more options in the lead in / out area ( eg extend/shorten path )

[Superman]

Originally Posted by driftmaster Hello. New here at the forums, i will probably find the answer in some thread but i'm too lazy right now =)

I should have come back saying, "sorry, I don't have the time, but you'll find that someone has already answered your query" LOL.

anyway, hope the answer helps

[driftmaster]

Superman, thank you for replying =)

I messed with lead in/ out but i'm still not satisfied..i think..First it position the tool at "X-7.502 Y1" And reads g41 moving to "G1 G41 D1 X-7.5 Y0."
I can get 1mm in X or Y but not both, how come? =(
Or is it ok to just read it in X or Y?
I think i read in machine manual it must be in both X and Y in order to work right..
Hmmf..

[Superman]

OK, let us go back to some sort of default settings

use 2Dcontour,wear, left, XYoffset=0
geometry = a straight line starting at X0Y0 to X100 Y0
tool #1 = 16mm diameter endmill, length off#=1, dia.off#=1

in the lead in / out dialog area
on "lead in" side
line tangent
line length = 50% (8mm)
arc length = 50% (8mm)
arc sweep = 90 deg

now click the arrow in the middle to copy data to "lead out" side
accept and re-generate t/path , now post this t/path
it should be similar to the following

G0 X-8. Y24. ( rapid to point )( start of lead in line)
G1 Z0.
G41 D1 X-8 Y16 ( lead in line- takeup comp.)
G3 X0. Y8. R8. ( lead in arc )
G1 X100. ( the actual geometry )
G3 X108. Y16. R8. ( lead out arc )
G40 G1 Y24. ( lead out line - cancel comp. )
G0 Z3. ( retract )

If line length has a setting of zero, this line will not be output
If either arc length or arc sweep has a setting of zero, the arc will not be output

A line by itself can only be "perpendicular" or tangent", if you want a line at a 45 deg approach, it is controlled by the arc sweep and the line will be tangent

ie tangent, line 55mm,arc 13mm,sweep 30deg ( try it )
now change tangent to perpendicular, then try a 90 deg sweep

this should all be viewable on the screen, your post may have some issues and we are trying to understand lead in / out at this stage

Your query "I think i read in machine manual it must be in both X and Y in order to work right.. "
Depends on your machine, compensation movement has a look ahead function ( it would be better explained in your machine's manual )

a rough example

a straight line from X0Y0 to X100 and taking up comp

X-20. Y0.    ( if D1 in control =8.0)
G1 G41 D1 X0.( goes to X0 Y8)( comp ON)
X100.        ( goes to X100 Y8)
G40 X120.Y0  ( goes to X120 Y0)(comp OFF)

[driftmaster]

Originally Posted by Superman OK, let us go back to some sort of default settings use 2Dcontour,wear, left, XYoffset=0 geometry = a straight line starting at X0Y0 to X100 Y0 tool #1 = 16mm diameter endmill, length off#=1, dia.off#=1 in the lead in / out dialog area on "lead in" side line tangent line length = 50% (8mm) arc length = 50% (8mm) arc sweep = 90 deg now click the arrow in the middle to copy data to "lead out" side accept and re-generate t/path , now post this t/path it should be similar to the following G0 X-8. Y24. ( rapid to point )( start of lead in line) G1 Z0. G41 D1 X-8 Y16 ( lead in line- takeup comp.) G3 X0. Y8. R8. ( lead in arc ) G1 X100. ( the actual geometry ) G3 X108. Y16. R8. ( lead out arc ) G40 G1 Y24. ( lead out line - cancel comp. ) G0 Z3. ( retract ) If line length has a setting of zero, this line will not be output If either arc length or arc sweep has a setting of zero, the arc will not be output A line by itself can only be "perpendicular" or tangent", if you want a line at a 45 deg approach, it is controlled by the arc sweep and the line will be tangent ie tangent, line 55mm,arc 13mm,sweep 30deg ( try it ) now change tangent to perpendicular, then try a 90 deg sweep this should all be viewable on the screen, your post may have some issues and we are trying to understand lead in / out at this stage Your query "I think i read in machine manual it must be in both X and Y in order to work right.. " Depends on your machine, compensation movement has a look ahead function ( it would be better explained in your machine's manual ) a rough example a straight line from X0Y0 to X100 and taking up comp X-20. Y0. ( if D1 in control =8.0) G1 G41 D1 X0.( goes to X0 Y8)( comp ON) X100. ( goes to X100 Y8) G40 X120.Y0 ( goes to X120 Y0)(comp OFF)

Thank you!
That made it!
Now the lead in and lead out is just like i wanted..

Thanks alot mate!

[Superman]

Great!!

I tried to give examples of what you can do by just altering the lead in / outs
Many create extra geometry, just to get the tool to drop in on a safe spot,
some times creating extra goem. is unavoidable, but I try keeping that option for the more difficult paths.

Steve

[driftmaster]

Hello again..

I have been trying X3 for a while now, now been trying to work out the cutter compensation again and got in to problems..

So Superman, or somebody else who is familiar with Mastercam..Help needed =)

Ok, so i'm trying to make a simple circle with cutter compensation inside the countour.

Withour lead in or lead out it posts :

"N40 G0 G90 G54 X14.978 Y1.M3 T225
N80 G43 H5 Z25.
N100 G1 G41 D0 X14.975 Y0.
N110 G0 Z5.
N120 G1 Z-34.
N130 G3 X-14.975 R14.975
N140 X14.975 R14.975
N150 G0
N160 G0 Z25.
N170 X14.975 Y0.
N180 G40 X13.975"

Here i can see last line is not like it used in mc9.0, it used to move in both X and Y while reading G40..Hmm, meaby its enough in X? don't know, havent tried in machine yet.

Not i try with lead in and lead out as i want to have more movement in G41 movement, now just 0.003 in X axis. (i got a alarm while ago because it didnt have enough movement..hmm)

Now it posts :
"N40 G0 G90 G54 X6.268 Y-12.021M3 T225
N80 G43 H5 Z25.
N100 G1 G41 D0 X6.975 Y-11.314
N110 G0 Z5.
N120 G1 Z-34.
N130 X12.632 Y-5.657
N140 G3 X14.975 Y0. R8.
N150 X-14.975 R14.975
N160 X14.975 R14.975
N170 X12.632 Y5.657 R8.
N190 G0
N200 G0 Z25.
N210 X-10000. "

So now im happy with the G41 movement but something is messed with the lead out part i think...What should i change or tweak?

I used the tool in mastercam x3 to upgrade my post processor from v9.0 to x3..

//

[Superman]

N40 G0 G90 G54 X6.268 Y-12.021M3 T225
N80 G43 H5 Z25.
N100 G1 G41 D0 X6.975 Y-11.314
N110 G0 Z5.
N120 G1 Z-34.
N130 X12.632 Y-5.657
N140 G3 X14.975 Y0. R8.
N150 X-14.975 R14.975
N160 X14.975 R14.975
N170 X12.632 Y5.657 R8.
N190 G0
N200 G0 Z25.
N210 X-10000.

N100 is a move to the start of lead in with cuttercomp using offset#0 ( most use the same # as the tool # for length and dia offsets )
(H0 and D0 usually are zero and are not changeable )
it then rapids down to the clearance plane, feeds into the job (note!! no feedrate applied - should be XY Feedrare on the G41 line , and Plunge rate on the Z)
N140 and N170 are your arc lead in/outs
you seem o be missings the lead out line and a cutter comp cancel (G40), without this you may get errors going to the next point

We have set our order of doing profiles as:-
-set co-ord system
-rapid to start point ( usually 1st point of lead in line )
-set spindle RPM , start spindle
-rapid descent to clearance plane and take up tool length offset
-coolant on
-Rapid to Retract plane
-feed to Z depth
-take up comp ( onto the 2nd point of lead in line )
-lead in arc ( if required )
-do profile
-lead out out ( if required )
-lead out line, cancel comp on last point
-rapid retract or do next depth ( depends on your settings )

Our Okuma's require a line to take up and cancel comp on

[driftmaster]

First, thanks alot Superman for taking your time and replys.

Now lets see, Feedrates are posted as should be, it was just that i didnt bother put any there because im just testing. But i tried, and its like it should.

Same with the D0, it was specified in tools and i changed it. Posts it like it should.

So ive been messing more with the lead out settings and it just wont work. posts the damn x-10000 everytime...

In v9.0 i havent seen this happen..

If i try to not use the EXIT in lead in/ lead out it posts
N160 G40 X-14.975 R14.975

But im not satiesfied with this neather..=(

Why won't it just make a simple move in x and y like it does when it reads the G41 code?

I had no issues in mc9.0 after your help..

Is this a error in post processor or what do you think?
I have no experience working with post processors...

[Superman]

OK, you're working with V9
can you make a test Mcam file with a circle and a line
and create operations to profile both using what you think is correct lead in and out ( so it looks good on screen )
-create a ZIP folder and place this Mcam file and the post you're using
-attach this ZIP folder to your next posting so I can have a look

Your on a FANUC machine , 3 axis ?
I think the X-1000 is set in the post , but I'll have a look first for you
I should be able to compare it to one of our V9 posts

Steve