verify 5 axis cut

[tedly]

When verifying 5 axis tool paths. The end mill went thru part when it is switching from one side to the other. Actually when cutting in machine it is working just fine because Z home first before table turn. I was trying a whole bunch of numbers in z clearance but it made no different. Does anybody know why? X2, X3 or X4 do this.

[gcode]

If you click

"Force toolchage" on the 2nd cut

Verify will do both cuts without rapiding

through the part.

You'll want to uncheck it before you post

unless you want a toolchange posted..

a lame answer.. but its all I've got

[tedly]

I am alway use force tool change on 5 axis move. for some reason in our post if we don't check on force tool change, we will have jerking moves even so c and a axis are unlock. so force tool change is there in this verifying problem.

[k turk]

this is a problem i come across pretty often - getting around the part between toolpaths without crashing. i frequently wonder what the best way is. A lot of times i will go in and write some extra code in by hand to manuever the spindle or i might segregate my toolpaths into different programs and run them separately. i've read some references to using lines as directional retracts, but i haven't figured that out yet.

 

_________________________________________

You'll want to uncheck it before you post

unless you want a toolchange posted..

_________________________________________

 

gcode, i don't think i get it - if you uncheck this before posting won't you be running into your actual part? maybe i am missing the point, why are you checking 'force toolchange?' to get a good verify result?

[MLS]

Verify does not simulate the actual way the machine will interpret the data. It may be right, but it may not. It also does not take into account how the post processor will convert the data to gcode.

 

If you want to be sure how the machine moves from one 5axis position to another, you can drive a curve 5-axis toolpath to manually control how it goes from one vector to another.

[k turk]

ahhhh, i think i see the lightbulb.

 

so MLS you are saying create a new and separate toolpath to move to and how you want to get from A to B? i have been thinking there was a way to reference this drive geometry in the original toolpath.

 

if that is what you are saying, it seems simple . . . . . and obvious, now that you've said it. of course, i have yet to try it. maybe not as easy as it sounds.

[Steve Hattori]

I've had this problem with mastercam's multi-axis routines for a couple years- only way I know to get around it is use only the "advanced"5-axis paths because they automatically write code to go around your part. The standard mcam stuf just outputs a single rapid move from the end of one pass to the beginning of the next one, and on my machine, it WILL go through the part.

Or, you can do as MLS suggests and make geometry. I don't know how you get that to work when the problem exists within a routine, and the tool goes through the part between passes. Works OK for going from one routine to another.

Sorry to not have a better solution.

[MLS]

As Steve is saying it will not work within a routine, only from toolpath to toolpath.

 

In my opinion it is somewhat of a workaround too because to me it would be greatly beneficial to be able to orient your lead in and lead out/ clearance vectors to your desire as to actually control this issue.

[bogusmill]

MLS came to our shop and went over some things that didn't seem right but still worked when I first started running 5 ax parts. He said the machine has at least 2 or 3 ways to resolve any tool vector and it can be hard to tell what your actuall going to get at the machine.

 

We do research work, not production so we operate somewhat different than most of you. One thing I've learned is to leave force tool change checked at all times. I've had near crashes trying to guess how far to retract between cuts and force tool change gives me the max clearance I can get. I've also seen what I expected to be a simple B axis rotation to the next cut turn into the head trying to flop over to the backside usually causing a crash but definately being uncomfortable to monitor. Those same cuts so far have remained on the operators side of the A axis when I added the force tool change command so It's part of my default definitions.

[Steve Hattori]

I have found that it also does this in a 4th-axis-roll toolpath- if the tool comes out of a pass, mcam just generates a straight line to the beginning of the next pass. If thats around 180 deg from the start, it goes right through the part!

 

do NOT ask me how I know.....

 

I can see this being endemic to a toolpath that you roll around a cylinder from a flat pattern, but there really is no excuse for it any 5-axis path. Its for that reason I do as much as possible with the adv 5x routines....

[tedly]

It may look like it's crashing into part in verifier but I can guaranty to you it works fine in real cut. Even so it run fine at the machine it doesn’t set good with me to see that in Mastercam verifier.

[Jim at Gentex]

Sometimes the home position specified in the toolpath parameters causes verify to gouge the part too. This happens to me sometimes, but the posted code is always good.

 

I'm not sure this will help, but it does happen.