Help!! Problem With Z coordinates in G code

[Socalsurferx]

Hello-
Our small company just recently purchased a new Haas TM-2 mill. We are all fairly new to the CNC machining area and need some help. We are trying to mill out a female die pattern out of a block of PVC Plastic that will then be cast into a different metal. The pattern is basically an open ended channel with some curve and shape to it. We designed the part in Solidworks and saved it as an IGS file and opened it in Mastercam X. No problems there, made the tool path and sent it to the post processor. One issue we had at first was the H and the T values didnt match up. Dont know how to change this in the program so I did it manually. The biggest problem is that we clamped the plastic down,went through the proper set-up procedures on the machine and start the machine and it wants to cut 6 inches or so above where it should be. I looked at the G code after and sure enough the line after the G54 line says Z6.018 which is the height of our stock in the program. the z should be clost to 0 or something i believe then slowly become more negative. the stock was not set up in Mastercam, the whole thing was drawn in Solidworks. Any ideas?

[SteveD]

Sounds like your part is not oriented right in MC. I too take files from solidworks (designer draws) to MC (V8 however). I find when I convert the file to MC the part is all out of wack & I have to re-orient it, my designer can't seem to figure out how to orient it right so when I convert it is where it needs to be. Check where you origin is in MC the part could be 6" above that causing it to right the code there.

[mishikwest]

Welcome to the wonderful world of mastercam.

first, what version of mastercam?

There is a parameter in the Haas control to alarm if H & T don't match. For learning the machine and mastercam, I'd recommend keeping that alarm on. H & T values either come from the tool or are assigned sequentially. Take a look at your job setup and see if "get values" from tool is checked. Then go and see what your tool def. is. Adjust either accordingly.

Sounds like your origin is not where you think it may be. Hit ALT+F9 and see where the blue crosshairs align. That is where your g54 should be set on the machine.

Yes when outputting from solidworks the planes get switched around..front in solidworks becomes top in mastercam, (at least if I recall correctly). If I have access to solidworks at the time (or can convince the part designer); create a new coordinate system and save the part as a parasolid and output that "new" coordinate system. When you open the part in MC, it will be oriented correctly. If you don't (or can't) go back into SW, you will need to either create a new view in MC, or translate your part to the top view. See how far that gets you, and come back if you need more help.

edit: Also sounds like your tool offest also could be off too.? In relation to the top of the part or the top of the table.

[dmealer]

Hello,
A few tips on the solidworks issue. I am constantly making parts in SW and importing them into MC with no alignment problems. First, when you design your part, notice the triad in the lower left corner of SW. Orient your part with the triad as you would in MC.
Never mind which plane it's on. Usually I just design it, the move it where I want using the insert, feature, move, copy command.
Also, in SW, make sure the origin is where you want to call X,Y,Z zero in mc.
The origin is not the same as the triad. When you start a sketch, you will see the origin in the middle of the screen. Once again, I usually just design my part and move it to the proper relationship to the origin after I'm done.
It takes a little practice, but once you get the hang of it, when you import your part to MC, it will be exactly where you want it from the git go, and only takes a min or 2 to acomplish.

Hope this helps!!!!

[Cammotion]

Originally Posted by dmealer Hello, A few tips on the solidworks issue. I am constantly making parts in SW and importing them into MC with no alignment problems. First, when you design your part, notice the triad in the lower left corner of SW. Orient your part with the triad as you would in MC. Never mind which plane it's on. Usually I just design it, the move it where I want using the insert, feature, move, copy command. Also, in SW, make sure the origin is where you want to call X,Y,Z zero in mc. The origin is not the same as the triad. When you start a sketch, you will see the origin in the middle of the screen. Once again, I usually just design my part and move it to the proper relationship to the origin after I'm done. It takes a little practice, but once you get the hang of it, when you import your part to MC, it will be exactly where you want it from the git go, and only takes a min or 2 to acomplish. Hope this helps!!!!

dmealer,

Not to hijack this thread, but I wonder why the triad Z axis is aligned with the front construction plane in Solidworks, and if there's a way to change that. You'd think that it would be aligned with the top construction plane.

[mishikwest]

The caveat is when bringing in parts from assemblies you'd have to save a copy of your part, re-orient, and then bring into mc.

I'd bet in an upcomming release of MCdirect you'd be able to output a coordinate system. It supports more and more features with each release.

[cadcam]

mishikwest which version of MC and Solid works are you working with?
I will be able to tell if you have the latest.And I can Check with CNC if they plan on implamenting the output a coordinate system. I use the WCS in MC to take care of how the part sits as with all types of files from Say Catia ,UG or SW they new put them were I want.

[Geof]

Originally Posted by mishikwest There is a parameter in the Haas control to alarm if H & T don't match. For learning the machine and mastercam, I'd recommend keeping that alarm on.

On Haas VF series it is Setting 15: H &T Code Agreement; On or Off