Floweline to output arcs in toolpath code

[Thee Rickster ™]

X4 MU1

 

I revolved a 1/2 rad to create a surface to

cut with a flowline using a 1/4"

 

when posting the code it generates without arcs

 

 

N120 T12 M06 ( 1/4 BALL ENDMILL)

N130 (MAX - Z2.)

N140 (MIN - Z-.6032)

N150 (TOOLPATH - FINISHFLOW)

N160 (STOCK LEFT ON DRIVE SURFS = 0.)

N170 G00 G54 X-4.6502 Y0. S12000 M03

N180 G43 H12 Z2.

N190 Z.1

N200 G01 Z0. F50.

N210 X-4.6484 Y-.1297 F250.

N220 X-4.6429 Y-.2607

N230 X-4.6336 Y-.3929

N240 X-4.6204 Y-.5262

N250 X-4.6031 Y-.6604

N260 X-4.5817 Y-.7954

N270 X-4.5561 Y-.9309

N280 X-4.5262 Y-1.0669

 

Is there any way I can get it to psot arc in the

XY plane using flowline?

 

Is it odd for the post to output line

movements on a perfect rad??

 

My buffer from dnc to the cnc catches up and

slows the path to a crawl.

 

Rick

[Tony35]

rickster

did you filter the toolpath and tell it to make arcs in XY?

[Thee Rickster ™]

No....where is the filter?

 

 

:EDIT:

 

Tool refinment is on I just checked a waterline

path. Is it supposed to be there for a flowline?

 

Rick

[Tony35]

under "total tolerance" in the finish flowline parameters

[Thee Rickster ™]

Found it, but it doesn't seem to work.

I tried one way filter/XZ/YZ/arc radius 0.05" to 2" then 4.05"??

 

It won't output the arcs.

Am I missing something?

 

 

Thanks

Rick

[Tony35]

did you try min arc rad of .005 to see if it will give you arc output?

 

do you normally get arc output on other toolpaths with filter on?

 

is the geo good? (not a spline)

[Thee Rickster ™]

Yes

Maybe.(do few like this) never really checked

It is a 1/2 rad/arc then surface/revolvee

 

If MC can't do it its ok. seems too easy. I just

exported the geo to another software and it codes it

with arcs as default, which make sense to me.

 

Just don't know why MC does it the long way.

 

Cheers

Rick

[Tony35]

did you try a different size tool to see if it would work? (.249 ball)

 

i drip off of ata cards so i dont really pay much attention to the code

 

where is peon to chime in on this

 

WAKE UP PEON!

[Thee Rickster ™]

The surface i am cutting is 8.3 Dia. why would

I need to take .001 off the cutter to get it to

post out arcs with the filter on?

 

i don't normally pay attention to the code either.

 

Guess the filter is broke.

[cunder]

When I use flowlin, and have the cutting method set to spiral, I do not see arcs output.

[Roger Peterson]

you have your slider set to 95% for cut tolerance, 5% for filter tolerance. your just not going to get any arcs with that tolerance setting.

 

You need to make your filter tolerance at least 50% of your total tolerance, preferrably more. (2:1 ratio before toolpath refinement worked well)

[Tony35]

quote:

---

why would I need to take .001 off the cutter to get it to post out arcs with the filter on?

---

i dont know why it just helped me in the past

 

quote:

---

you have your slider set to 95% for cut tolerance

---

good point i missed that im so use to to how i have mine set

[Thee Rickster ™]

Roger, I guess I don't really understand the settings, very well.

 

I can't try it now as I am on another rush job.

I will let you know when I have the time.

 

Thank you

Rick

[Roger Peterson]

In the Tolerance distribution section:

 

cut tolerance + arc tolerance = total tolerance

 

you have:

 

cut tol (95%) + arc tol (5%) = total tol (100%)

 

move the slider bar (or type in different values) between the cut tol and arc tol fields so they both say 50% and see what kind of results you get.

 

 

Regards,

[Thee Rickster ™]

Cool

 

Thanks

Rick

[kunfuzed]

This has happened to me as well. Noticed it on a Catia solid, but also tryed it on a revolved surface like you with the same results. Mine would go from arcs to lines to arcs though. I'm very aware of the code, as we run haas here, which don't handle tiny segments very well.

 

+1000 for asking this! What gives?

[Colin Gilchrist]

Rick,

 

You can disable the new toolpath refinement function and use the old style toolpath filter. I find this to be much easier to use. The toolpath refinement is nice for producing smoother toolpath motion on complex surfaces though.

[shazam/TPP]

anymore news on this one? i have my filter set at 2 to 1 but still receive lines instead of arcs.

[Thee Rickster ™]

Colin, I've tried every thing.

 

It is a plain round surface. You can try it on a cone

and use a ball cutter and still MC chooses not to post arcs when it should on simple round surfs

 

I called a friend to test it in 2 different software's he uses and both put out arcs..??

 

Filter must be broke.

[Thee Rickster ™]

Roger, your slider method made no difference.

[Mgrenier]

Just a thought here,

 

Is you control definition configure to allow arc in all the planes? It did bite me before.

 

HTH

[Thee Rickster ™]

Marting

 

Yes it is

[Dennis at CAD/CAM Consulting]

You MUST have more tolerance in the arc filter than the toolpath to get arc output from the filter.

Set it so you are using 40% of the total tolerance for toolpath and 60% of the total tolerance for arc filtering. Even 50/50 will most likely yeild no arcs.

[Troy Gossett Indepak Inc.]

Rickster I'm seeing the same thing here with scallop TP tried all suggestions above. Now where do I shut it off at? I know there was a switch in MU1 can't find it in MU2.

Edit: Found switch in Control Panel Applet.

 

[ 12-14-2009, 01:40 PM: Message edited by: Troy Gossett Indepak Inc. ]

[Clarence L Cook]

My solution to the no arc output for finish flowline is setting the cutting method to one way.

 

I have a cone surface that I created in an earlier version of Mastercam and I brought it into X4. I changed the cutting method to spiral and I get a whole bunch of line moves.

 

Hope this helps.