PDA

View Full Version : Feeding On 3d file



jamesr
12-06-2006, 01:33 PM
Im runnig a 3d z-finsh pretty simple 3d just some diameters the problem im having is when feeding around it slows way down in areas then back up to my normal feed which is 65.000 slows down in some areas to 25.000 any ideas why this happens?

Thanks
James

Ed_R
12-06-2006, 01:38 PM
Its' probably due to the huge number of G-code commands your 3-D file requires on the curves and stuff. Seriously! Ger21 pointed out to me a long time ago that in one section of my code, it was taking 2000 lines of code to cut a pocket through the Meshcam output, where it could have been done in 8 lines.
I'm no expert but that would probably slow anything down;)

hoss64
12-06-2006, 06:14 PM
Is your post generating a G9 code in your program? That code slows your feed down when you get into tight radii, or corners. If so, change it to G8 to solve the problem.

championp
12-06-2006, 09:47 PM
You could adjust your surface tolerance to a larger number to get less code. You can only go so big before it starts to give you a faceted finish. Our's defaults to .001" but for really nice finishes and more details I go as low as .0002" on the surface tolerance. this setting is under the "cut control" tab in your z-finish menu.

Chris

planar39
12-07-2006, 06:42 PM
i typically see this on a 1985 era machine with low memory and a person is running direct (dnc). my mill can hold 80k, running direct it pulls in 4k at a shot to 2 buffers, however our older fanuc 11m makes all sort of jerky motions when-heres a good example- machining a dish shape in a 24"dia piece of nylon. when we told it 110 ipm, were lucky to see 65. You could add more bubble memory but very expensive i hear, and the amount of memory would be like 2k or somthing pathetic,(assuming you have a 1985 fanuc 11m)

raise curve tolerance to .002 and see if you like the finish
ed proposes somthing i know nothing about, another way to post? tell me more!

camaru
01-24-2007, 04:56 PM
I do not know for sure but maybe you could use the arc filter option on the post page. It will take a series G1 line moves that are on a plane, XY, and if those points can be converted to arcs it will do that. The benifit of arcs in tool path is that it is easier for the machine to handle and the machine should run more consistantly.