Surface Rough Parrallel

[Festus]

hmmmm. i could swear when i used to use this toolpath that i could rough one side of the part before it would retract over to the other side. i can't keep it from retracting over the part along each slice. been buggin' me for a while. am i overlooking something simple?

 

note: i don't see any difference when i check "optimise cut order" and i'm sure i used to in X4?

[K2csq7]

Screenshot? I usually use 2 ops for something like that...

[Festus]

screen shot

[K2csq7]

How about Containment Boundaries?

[Festus]

i am roughing this mold out of a 18" x 27" x 11" block. it needs to cut over the whole part. am certain that with X4 if i checked the optimise option i would get almost no rapids? i will fire up X4 and see what results i get. On parts like this i'm always afraid i'll run out of air in my shop since we're cutting so much air!

[K2csq7]

On parts like this i'm always afraid i'll run out of air in my shop since we're cutting so much air!

 

Nice!

 

Sounds like a job for one of the newer toolpaths, 2d high speed core mill or optirough...

any reason your sticking to parallel?

[Hardmill]

Is the cut from both sides switch on ??

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[Festus]

tried high speed. looks good in verify but takes forever on the machine? Would like to use the optirough but the fact that i cant get it to zigzag so it takes me way too long?

 

I like the parrallel 'cause it sets up my finish passes nicely! i'm cutting foam or MDF so i can allow negative plunges with no worries. The optirough works real nice as well. just takes to stinkin' long!

[mayday]

i'm cutting foam or MDF

What a life !

 

I'm stuck cutting complex surfs in Inconell, Rene, Hanes, Ti-Aluminide

an Orange glow is normal round here

[K2csq7]

:Hijack:

What a life !

Seriously

Just got done with this friggin thing in age hardened Waspaloy, .002 clearance in front of the insert & .004 behind the blade. Had to make the tools myself cause nobody would even quote the *($@#(* things... The blade thickness is like .055" :lol:

:Hijack over:

[Festus]

What a life !

 

I'm stuck cutting complex surfs in Inconell, Rene, Hanes, Ti-Aluminide

an Orange glow is normal round here

 

some of my parts still have about 40 hours cutting, frontends of buses, marine consoles, ect. my other shop cuts wood production parts.

[Festus]

Is the cut from both sides switch on ??

 

no...i'm using allow multiple plunges. less rapids

[Festus]

:Hijack:

 

Seriously

Just got done with this friggin thing in age hardened Waspaloy, .002 clearance in front of the insert & .004 behind the blade. Had to make the tools myself cause nobody would even quote the *($@#(* things... The blade thickness is like .055" :lol:

:Hijack over:

 

 

I've only been programming about 2 years so i have a lot to learn still!

[Roger]

I tried a quick similar shaped part in X5, and X4, with optimize cut order on and off. Same-Same. If you change the machining angle of cut from 90 degrees (Your tool path) to 0 degrees, theres a big difference in rapid moves.

 

I would like to know what you find out on this.

[MotorCityMinion]

"I've only been programming about 2 years so i have a lot to learn still!"

That being said, the part appears to have quite a few steep sloped facesand I'm not so sure that rough parallel is the way to go here. IMO, HST core roughing with a trimmed tool path, should produce a more efficient tool path.

 

"If you change the machining angle of cut from 90 degrees (Your tool path) to 0 degrees, theres a big difference in rapid moves."

 

You can dial it in a lot closer. Find the angle that those faces are at and add 0.00 or 90. to that angle.

 

 

 

[Festus]

minion...I did in fact change the angle. What is hard to see on the snip is the islands and trim ledges on the inside of the part i've been playing with the high speed paths, but haven't been able to beat time on machine? also the high speed paths are an issue with my machine having a 41" Z heigth. the sudden changes in direction within the paths are causing quite a lot of runout?

[Festus]

minion...is there any specific settings in core roughing that are key? keeping in mind that i need to maintaain that slope somewhat for better clearance?

[MotorCityMinion]

HST core should provide ample clearance. HST area should also work with containment boundaries and/or some dummy surfaces and might provide less air time. Left it fly without trimming or boundaries and it will waste some moves.

 

"the sudden changes in direction within the paths are causing quite a lot of runout?" Perhaps adding fillets to the tool path will smooth it out some. You can also try to set your stock to leave on the walls at about 70% of the cutter then attack the remaining stock with waterline. Sometimes, one roughing tool path just doesn't get it.

 

Runout??

 

Can you upload the file as a X_T or step?

 

 

[Festus]

Can you upload the file as a X_T or step?

 

the file is too big? even when zipped

[Gary]

What speeds and feeds does the machine have? We cut this material also for check fixtures. highspeed area clearance with 70% stepover .3 step down and 300-400ipm works good on our haas. If you select min vertical retract with "output feed moves" checked it does a good job of not jumping all over the part and having lots of retracts.

[MikronGuy]

did you try the surface flowline the tool does NOT jump around much and finishes one angled before moving to the next. watch the surface normals. the bigger the gap settings the less the tool jumps around and the less air you will cut

[Festus]

micron...I use flowline a lot for finishing... however i have a lot of flowline issues when i have to select many surfaces?

[Festus]

What speeds and feeds does the machine have? We cut this material also for check fixtures. highspeed area clearance with 70% stepover .3 step down and 300-400ipm works good on our haas. If you select min vertical retract with "output feed moves" checked it does a good job of not jumping all over the part and having lots of retracts.

 

For roughing I use 2" stepdown with 40% stepover at 500ipm because of the big stepdown I have issues with my holder hitting if i don't use something like parallel or optirough I can also get it to not jump around, but because of the lack of a zigzag option in opti it just takes too long

[JDowe]

Try this

Cutting "one way"

Cut both sides

No z motion up or down

gap setting optimize cut order

[JDowe]

Try this

Cut one way

cut both sides

no z follow motion

gap setting optimize