Unable to determine a valid machining zone

[Thee Rickster ™]

High Speed Surface Finish Scallop, Rest Material.

X2 SP1

 

(waterline works no problem)

 

I seem to get that error when I try to use this

path, often. I have been using the same geometry

and boundaries all day.

 

Does anyone have a solution for this error?

 

Thanks

Rick

[Ocean Lacky™]

save file, close and restart mastercam, regenerate seems to work for me

[Colin Gilchrist]

Run RAM saver, and check your cut depths.

[peon]

Did you copy and paste a previous toolpath? Try making a new toolpath with the same parameters without restarting or rebooting. This usually works for me. I also use ramsaver on every other toolpath.

[Thee Rickster ™]

Ocean

 

that worked.

 

Colin,

 

What so you mean by cut depths?

Increasing cut depths will give me an undesirable

surface finish.

 

I am a lil' afraid of Ram saver...i lost geometry

once and well you know.

 

Why do you lose geometry, used in tool paths, when

you use Ram Saver?

 

Thanks for the speedy replies.

 

Rick

[Ocean Lacky™]

[chipking]

I am having the same problems with the SHS (scallop rest pass) and just plain trying to have it run a high speed scallop pass. Tried everything that I know of so far and the help listed above, but it's (more me) not click'n. Any other help would be great, I will probrobly go back to using a plain scallop toolpath with check surfaces to keep the holder away from the tower I am machining around.

[Thee Rickster ™]

Check yer Cplane and Tplane make sure they are

correct

 

in the tool path parameters:

 

Check your steep/shallow, the min an max depth.

make sure your clear and retract are above the

min depth and your geometry is under the min. also.

 

In Planes(wcs) make sure the 3 are the same

 

Axis control is on 'no-rotation'

 

Above all else make SURE you coffee cup is full

 

HTH

Rick

[chipking]

I have it all set the same way as you say but it still won't work. I tried it as a rest mill with the same size tool- won't work there. Then I redid it with a smaller tool and 0 stock allowance, it would go to the part but is would not cut and would go right back up. I can get it to ruff but cannot get the scallop to cut!!! Thank god I am drinking beer after work!!

[chipking]

Just relized I don't have SP1 loaded...does that make a difference? Going to do it now.

[YoDoug®]

Often when I get the "unable to determine a valid machining zone" I fix it by going in to the steep/shallow and hit the find depths button, then I re-enter the actual depths I need. This works most of the time.

[chipking]

Guys, thanks for all the help but it's still not working. I'm going to put it to bed for awhile and stick to the things that work. It's amazing how pissed one little thing can get you!!!I need to smell the flowers for a awile!! Thanks once again.

[Thee Rickster ™]

Doug's suggestion has worked once for me also.

 

I also rectify the problem by making a new

identical path and then delete the old one.

 

Sometimes the one with the problem cant be adjustd

to ever work again.

 

can you emsil me your file or put it on the

FTP site? I will gladly try to help.

 

Rick

[chipking]

I will see what tomorrow or Monday throws at me and I will contact you then. Thanks

[Thad]

quote:

---

What so you mean by cut depths?

Increasing cut depths will give me an undesirable

surface finish.

---

Check your cut depths (not depth cuts) and make sure the numbers make sense. For example, if you have surfaces between Z0 and Z3. and you're cut depths are from Z5 to Z4, you'll get "unable to determine a valid machining zone."

 

Thad

[edmBosto]

quote:

---

I also rectify the problem by making a new

identical path and then delete the old one.

 

Sometimes the one with the problem cant be adjustd

to ever work again.

---

That has happened to me in wire edm many times.

Only once or twice in mill. In wire I would need to constantly edit programs because of day burns vs night burns. You start taking a large job in the wire and constantly edit the paths and after awhile it don't likey.

[sharles]

quote:

---

quote:

--------------------------------------------------------------------------------

I also rectify the problem by making a new

identical path and then delete the old one.

 

Sometimes the one with the problem cant be adjustd

to ever work again.

---

+1000

 

Rickster,

 

why are you afraid of RAMsaver? I use it all the time, and I have NEVER lost any surfaces, but I make sure to NEVER tell it to delete any duplicate surfaces.

[Thee Rickster ™]

Lets just say it cost me a lot of time in the

X2 days. I had to work on my own time, NOT the

software developers, to replace the loss time.

 

My files are 2 to 300 meg, always, and no way will I chance it again.

 

X2MR2SP1 seems stable without using 'RAMsaver'

so I will let it sleep in the backround.

 

Is Why.

[Thee Rickster ™]

Today I had a High speed Scallop path that I can

not get to work with this error.

After an hour of trying everything I ended up using surface finish parallel to suffice.

 

Even recreating the boundary and making a new path

could not get the scallop to work??

[sharles]

Rickster,

 

it sounds like you are working with files approx. as big as mine. When I have had problems getting my surface scallop toolpath to run, I do one of 2 things. My default for filter is set to .001. So sometimes I simply bump that up to .0015, and then it will calculate. The other thing I do is split my part in half and make 2 finish scallop programs. My guess is the scallop program takes so much ram that even though I have 4gig of it, it's not enough. Normally one or the other work around will get me a good finish program with .03 step, 0 stock.

[Thee Rickster ™]

Sharles,

 

ironically I got it to work for the 1/4" ball

so I picked the cutter I wanted 1/8" ball and

nothing would make it work.

 

i am going to try and save as the file and delete

everything except what I am trying to do.

 

I let you know how it goes

[Thee Rickster ™]

nope, that didn't work

 

I guess MC picks and chooses what it wants to cut.

 

it works for most geometry

 

Now I am only giving it one try and go back to the

old parallel paths.

 

Rick

[Thee Rickster ™]

I have come up with somthing:

 

When I made a boundary a rectangle it worked.

When I put 1/2" radius on the rectangular

boundary it worked.

 

When I changed 1 of the 4 radius to 1" it gave

the error.

 

I wonder if that is a bug.

[Thee Rickster ™]

chipking

 

I xform/copy project your profile to z8.5 and tried that bnd, did not work.(then deleted it)

 

I created a rectangle from scratch the exact size

yours with the same rads to exactly match your

profile 1/2" above your original, did not work.

 

I offset contour your original profile .001"

larger and it worked.

 

I offset boundary I created above yours and

it worked

 

I have no idea why it won't take the orig profile

or a new one i created exactly the same.

 

 

Rick

[chipking]

I have not had a chance to work with the file yet but THANK YOU!!!