[Robert M]

Wondering if there is a way I can « see » before actually machining / cutting a part, what refinement, if any, the change made in the Arc Filter / Tolerance in the parameter box
Read a few time the help, I can…sort of…understand…but the results is….not to my liking, only to be seen after test cut !?
Anyway I may see it somehow before cutting, minimizing time & material, so one can correct it before….test !
Thanks

[Superman]

What I have done....
is set backplot to display different colors for a linear moves & arc moves
- depending on your version
--> backplot --> options
leave the lines as green, set CW & CCW arcs as red

Your Filter settings must not be OFF
- in the control file, arcs must be supported (and enabled ) in the appropriate planes ( that your machine can handle )

[Robert M]

Thanks again Superman.....I'll try this and give my feed back later.
You have come to my rescues ...again, thks

[Robert M]

Need some further assistance....
Filter setting of.... Where to go to do this ?
I've search, but never played with this, can't seem to grasp where it is !? may you help !!
Arcs are checked appropriately though !
colors are changed.
Later

[Superman]

Need some further assistance....
Filter setting of.... Where to go to do this ?
I've search, but never played with this, can't seem to grasp where it is !? may you help !!
Arcs are checked appropriately though !
colors are changed.
Later

Depends on the Mastercam version you are running....& what operation you choose. to what it looks like
- generally it is called "Filter" or "Tolerance" ..& it is a part of each operation

It is now a slider bar type of function ( X7 onwards )
it allows Mastercam to "fit" a toolpath to a 2D/3D shape within a defined band
- there is an NC output side also that allows the post to "fit arcs" ( also within a separate band to eliminate excess points) to adjust those toolpaths to get arcs
- these two band-widths add up to be the total tolerance that you can input.

- it may ask for 1:1, ....this is the same as setting the slider to 50% cut--- 50% NC ....in all cases the final NC toolpath should be within the "Total Tolerance" band
there is checks below to what planes you want to allow arcfit
----this is trial & error , and would depend on the purpose ( & quality needs ) of the part being manufactured

[Robert M]

Hi ....SuperMan !
They say...better later then...not taking care of it !?!
I've been just to buzy, so I had to push aside this situation / learning curve !

Back at it !
I may have expressed my self no correctly !
I got this "filter setting" ( see pic)
Attachment 267830

But still cann't realy see any changes in "verify" ?
Is this "only" for 3D toolpath....or I should see it in 2d also ?!
Cauz, when I change the colors setting
Attachment 267834

I still can't see any of the new "toolpath" color setting??....i only see the "loop colors" setting ??
Attachment 267840


Hope this make sens....
Help.....I'm lost ?!?! :drowning:
PS....Using MCX-7

[Robert M]

Here’s another perspective of why I’m asking all this !!
Had a commission work to be done and the output was not satisfying enough out of the CNC router !
Usually, this kind of “minor” cut goes …ok !
This time, it came out with “scallop” marks on all panels cut, and the interesting ( puzzling for me !) part, all where cut in multi passes CW and a final CCW pass at a very conservative cut ( 0.075”) with a slow feed & speed (with a new end mill)!
All tangential cut shows LOTS of scallops, but all linear ( vertical & horizontal) are fine !!

Here’s some pics to put an image to all this !
Tangential cut :
Attachment 267928

Vertical cut :
Attachment 267930

What I’m trying to find before trouble shooting the mechanical aspect of this, is I’m hoping to see the programming side of it 1st.
I have a “feel” it’s the program as all panels are showing the scallop marks at the same location if you stack them on over the other, although, none of them had the same “exact” starting physical point, meaning, the board where put on the CNC table at different location, then the 0.0 set at each !!
This is why it make me go….hummm !!

Thanks for any help !

[slowlearner]

Question,
Were the chatter marks there before the finish cut?
Although I am not a machinist I was always told to climb mill.

[Robert M]

Hi....
It make no difference as the the cuts "before the finish cuts" are done in a rough toolpath strategy and in climb ( CW)
For best finish, small increment in conventional (CCW) direction is best !

[jeffrey001]

Can you post the part of the program that is the problem?

Is this a large radius cut or a straight line?

Jeff

[Robert M]

Herewith a photo to tell more :
Attachment 268006

And the code :
Attachment 268008

Thks Jeff....and all others

[jeffrey001]

OK, looked at you code and look to be OK.

I think this sound more like a mechanical problem, maybe backlash or loose bearing on the X axis.

Normally, filter setting is for 3D toolpath, not for straight line or if the CAM output curve as many many lines of code.

You could try to rotate the parts in Mastercam to have both sides of the part at the same angle as those with the scallop marks and I'm pretty sure those scallop marks will be on both sides of the part but not in the middle of the part.

Jeff

[Superman]

I got this "filter setting" ( see pic)
Attachment 267830

OK...Turn ON your "Line/Arc Filter Settings....& have the XY(G17) ON
---- this allows the operation to "Fit Arcs"
---place the slider at the 50/50 ....same as the old 1:1 setting, this allows Mastercam to adjust the calculated path to create arcs....& allow the post to also adjust output.....but the final output not to exceed the "Total Tolerance"

Hi....
It make no difference as the the cuts "before the finish cuts" are done in a rough toolpath strategy and in climb ( CW)
For best finish, small increment in conventional (CCW) direction is best !

Looks like wood being cut - many factors affect finish
Tooling
- tool selection....sharp & stiff as possible ( no flex ) ( 2 flutes can be big source of flex, use 3 flutes or more )( hi-helix single flute may be stiffer than a slot drill )
- tool stick out....short as possible
- RPM & Feedrate.......maximum feed before machine starts cutting corners, then work backwards to get feed per tooth, and then set the RPM to those feeds
- Climb mill (CW ) will make the tool flex away from a part, not bite into...say a corner,,,, but downcut tooling may perform better in conventional ( CCW) direction, only you can prove the better method
- width of finish pass

Machine
- rigidity of the Z axis
- backlash of ALL axes
- belt flex on XY axis drives

Material
- swarf / chips.... make sure tool is not re-cutting or jamming up.. recutting tends to create more heat & blunt tools quicker.
- use vacuum / air whenever possible.....air would cool better, but make a larger mess
- softwoods & hardwards would have different cut parameters / methods

Suggest you use a stiff tool to finish, do one in 2 depths & the other in 1 pass, play with the finish allowance , compare results
- also...finish 1 piece to 3/4 of it's depth.....this should leave a step & show that the finish tool has actually cut something

Nothing is meant to be easy

[Robert M]

I think this sound more like a mechanical problem, maybe backlash or loose bearing on the X axis.
Same initial thought I had till I notice all 6 cut panels have the same scallops at the same location and that goes to say, the "blank" panel were not set at the same initial starting point ( o.o ).
you'd think if it's mechanical, it would show some variance ( scallop location marks) between cut panels ??!!

Normally, filter setting is for 3D toolpath, not for straight line or if the CAM output curve as many many lines of code.
That is the other reason of my help request on this thread, is I'm hopping to see in verify the changes I make in Arc filter section. Because the output code does change when I change the setting in that field !?

I truly realize that eventually I will have to "troubleshoot" the mechanical aspect of the machine also, but before going there, I'm hopping to zero-in, to...confirm, the "computer" part of the equation.....plus, It would help me for further usage to find out how to see, in 2d cuts, the Arc filter changes before actually going at the cut. The main reason for this verify !!

[hoffmannm]

Wouldn't your arc filter settings change nothing on your "Tangential" cuts? those are straight moves not arc'd.

As for whether you can see your arc filter settings reflected in the verify playback, I dont know, but I would assume the quality of the playback is primarily determined by the quality slider inside verify.

[Robert M]

OK...Turn ON your "Line/Arc Filter Settings....& have the XY(G17) ON
---- this allows the operation to "Fit Arcs"
---place the slider at the 50/50 ....same as the old 1:1 setting, this allows Mastercam to adjust the calculated path to create arcs....& allow the post to also adjust output.....but the final output not to exceed the "Total Tolerance":

Did this part too....plus all suggesting before....and still can't see ( the changes) it in verify ?!

Sam as :

But still can't really see any changes in "verify" ?
Is this "only" for 3D toolpath....or I should see it in 2d also ?!
Cauz, when I change the colors setting
Attachment 267834

I still can't see any of the new "toolpath" color setting??....i only see the "loop colors" setting ??
Attachment 267840

Hope this make sens.... ??

[jeffrey001]

Do you think you could post a video when you're doing the cutting?


Jeff

[Robert M]

See Jeff, although I appreciate understanding what DID happen, my goal here is further to understand how can I ( or any other for that matter) avoid & see in verify some Arc Filter setting changes before the actual cut.
My specific scallop trouble is a past trouble, no longer in process, therefore, I will not make anymore of this cut....and no offence, will not go there as to much other work waiting !!

For further reference and future need, I'd like to know if it's possible to actually see in verify the different setting made as a comparison....like a before & after....before making the actual cut, before the...OUPS..darn NOT GOOD !

I know and understand I may have ALSO other issue, like some mechanical ones ?!
AS SUPERMAN explained better then I could....

many factors affect finish
Tooling
- tool selection....sharp & stiff as possible ( no flex ) ( 2 flutes can be big source of flex, use 3 flutes or more )( hi-helix single flute may be stiffer than a slot drill )
- tool stick out....short as possible
- RPM & Feedrate.......maximum feed before machine starts cutting corners, then work backwards to get feed per tooth, and then set the RPM to those feeds
- Climb mill (CW ) will make the tool flex away from a part, not bite into...say a corner,,,, but downcut tooling may perform better in conventional ( CCW) direction, only you can prove the better method
- width of finish pass

Machine
- rigidity of the Z axis
- backlash of ALL axes
- belt flex on XY axis drives

Material
- swarf / chips.... make sure tool is not re-cutting or jamming up.. recutting tends to create more heat & blunt tools quicker.
- use vacuum / air whenever possible.....air would cool better, but make a larger mess
- softwoods & hardwards would have different cut parameters / methods

Suggest you use a stiff tool to finish, do one in 2 depths & the other in 1 pass, play with the finish allowance , compare results
- also...finish 1 piece to 3/4 of it's depth.....this should leave a step & show that the finish tool has actually cut something

Nothing is meant to be easy

[jeffrey001]

https://www.youtube.com/watch?v=Ws9gRlJ-9eY

You won't see any change in verify when playing with arc filtering in a 2D toolpath.

Your post will always output I and J or R when doing 2D toolpath. No change on G01 move too

In 3D toolpath, most of the time, the post will output many straight lines instead or arc so when you adjust the arc filtering, you will instruct the post to adjust the lenght of those lines depending on what finish you want and how long you want the Gcode to be.

Long lines = smaller Gcode = rought surface = Faster roughing operation
short lines = bigger Gcode = good finish = Longer finish operation

If you look at the picture, the space between straight lines and the radius the tool is suppose to follow, this where the arc filtering will be important, this will determine the finish of the part surfaces

Hope this help and hope I understood you question.

Sorry, english is not my primary language

Jeff

[Robert M]

Sorry, english is not my primary language
What is...le français ?!