X2 5ax question

[Jimmy Galto at SAR Engines]

I programmed a 5ax multisurf toolpath around a feature and when I go to run it, the tool goes for the wrong side of the part. This feature is repeated around the part several times. I used the regular 5ax multisurf and the advanced with no success. The odd thing is the two programs posted out with different angles both going to two different features, neither of which is correct or the same. The values are not 180 off either and inverting the angles doesn't help.

 

Earlier I ran a 3+2 toolpath which was right on location, angles and all.

 

What am I missing here?

[Guest]

Have you checked your surface normals?

[Jimmy Galto at SAR Engines]

Yes, they appear correct. I was doing some checking and the feature it's attempting to machine is 180 degrees away from the one I want machined.

 

The posted angle is 40 and by eye it appears to be very close at 220.

[Travis_Buchanan]

Are you using solids? If so maybe select from back was active. Did it backplot correctly?

[TonyNanni@BNB]

are you using a NAMED WCS. MCs multi axis tool path only uses the original world coordinate system. If you are programming multi axes tool paths the cad model must be moved to the machine position. you have to have the fixture layout done ahead of time and the cad x,y,z zero has to be the center of true rotation. The machine kinematics must be known ahead of time.

[Jimmy Galto at SAR Engines]

Backplot looks good. My cad file and machine setups are identical. I also have the axis of rotation and 0 deg. positions set correctly in machine definitions manager. I've decided to just program some 3+2 toolpaths to see what kind of positioning I'm getting. These are set from named views and look correct in backplot and verify. When posted though, the angles the machine moves to are not correct to place the tool on the feature I want to machine.

 

I tried changing the direction of rotation with no success. Is the primary direction the positive or negative direction?

[Jimmy Galto at SAR Engines]

My first statement about the angles being correct with 3+2 machining were actually correct by coincidence. Due to the spacing of the features and the direction of the named view the angles happened to be the same. When I tried a full 5ax program the problem became apparent. Also the 5ax program was done in the original WCS, no changing of views or tool orientation.

 

Know that I've changed the view and tool plane to a different location and attempted to make a 3+2 program, the angles are not correct.

[crazy^millman]

Ok are you using WCS top only for your 5 axis programming??

 

This comment will problay be disagreed with, but I never use anything other that TOP WCS for all 5 axis programming. I ONLY use C-planes for my axis or vector control for my 5 axis machining. Is this the way the part is programmed?? If you would like to email me your file I would be glad to take a look and see if I can see anything out of place.

 

One thing I will say is to me a problem with Mastercam is what you see in Backplot with 5axis is sometimes nothing like what you get for posted code. If your X is not adhereing to the right rule for the machine(IMPORTANT TO THINK OF THE MACHINE) then it will back plot correct all day long and post and not give you an error but once you get it to the machine (unless you have a verfication program) will you see the problem.

[Jimmy Galto at SAR Engines]

Millman,

 

You have mail, thanks.

[crazy^millman]

You have mail. When doing your 5 axis toolpaths leave your C-planes at Top as well. I never move my cplanes when doing 5 axis either. I will move them for 3+2 which tels me you were doing them right, but if you were using them for 5 axis toolpaths the same problem I explained to you about WCS and 5axis will happen if you use C-planes and 5 axis as well.

 

HTH

[Travis_Buchanan]

Crazy^Millman wrote......

quote:

---

This comment will problay be disagreed with, but I never use anything other that TOP WCS for all 5 axis programming. I ONLY use C-planes for my axis or vector control for my 5 axis machining.

---

Is there another way?

[Fig sign]

i TEnd to agree with Crazy^Millman

I never use Wcs at all ,always c-plane and tplane and WCS off

Found a couple of issues with WCS

[TonyNanni@BNB]

I don't understand. is the cad origin lined up with the physical machine setup. if not you have to XFORM the cad to match exactly to the center of true rotation. you have to know the machine kinematics and how the part is fixtured on the machine. MCs multi axes tool paths don't use Named work planes or WCS, you can't mix and match. You can use named work planes for 3+2 tool paths but there can only be one WCS and it has to be TOP. all operations have to use WCS TOP.

[Nils N]

Tony in 5axis you create your tool paths with the WCS and T/Cplane always set to top, you can have the part any where within your machine parameters. For control of the axis use your parameter's and or tool path section to control the tilt or follow vector lines. It you crate your tool path in a different plane you have problems. +1 to Millman

[Jimmy Galto at SAR Engines]

Thanks everybody. With your help, actually found an issue in the post which was corrected. I appreciate all the input.

 

Thanks