[ScoobyDoo]

:drowning: WE use FeatureCam for our CNC programming. Can someone tell me why every now and then the cutter path will stop and cut a perfect circle into the job (usally scrapping the piece)?? This only ever happens during the roughcut. WE have HAAS's, Bridgeports and JohnFords and this has happened on all of them at one time or another. The problem is that this circle cut does not show up when you view the cutterpath in FeatureCam but is obviously being posted out with it!!! The last time all we did was load the surfaces back in as iges instead of step and the circle cut went away???????

Any help would be greatly appreciated!!!

[Wiseco]

Check your post precessor. The code simulation of the work isn't from the code post.

Sorry to not helping you more, my english sux.

[HuFlungDung]

I would advise you to set your post processor to output maximum of 1/2 a circle per command. This is for the sake of the controller, which can sometimes be fooled by the ambiguity of a full circle command. Use I and J coordinates for the same reason, rather than R, to define the arc center.

[GisMo]

I know your problem! I had the same problem. I don't know your control, but I had an Anilam controller and it would put circles in the middle of the contour. This happened because: The arc length featureCAM programmed was too small for the controller to compute and the resulting output is a cicle. You can adjust your post processor with an if statement getting rid of the small arcs, or in the post settings there is a min arc length, i think default is .0001 make it .001(try this first) and you will be fine. You can always adjust your profile you are machinng. I noticed it occurred when the geometry was created from a spline rather than an arc. Let me know if this helps you.


GisMo

[ger21]

We get this with our router sometimes, due to rounding errors I think. I usually change the endpoint in the g-code by a very small amount (.01mm) and it will usually correct it. Probably not an option for you. If you're using R arcs, switch to I, J arcs and it should go away.

[NC Cams]

My EZTRAK would cut great circles, inside or outside with the OEM canned code. Yet, when we tried to do a circle with G code, it would puke.

So we tried half circles where it did the first half and then puked in same half. Tried 1/4's same deal.

Yet, if we do a cam profile (3/4 of a circle with an external bump0 , at point to point milling with G code at 4 or 8 cuts per degree, we get stuff so deadly close to a CNC ground part that it is nbelieveably scarey.

CNC machines, you can't see how they think, therefore you can't trust them.....

[MarshCustom]

I had the same problem this week on my Bridgeport CNC. The problem was from having cutter comp on and not giving it a linear and arc move before it started the cut. A Rep from Feature CAM was in this past week and said the problem was in the Bridgeport. I put a move above the part then drop down and start the real cut. Hope this helps.

[NC Cams]

Keep one thing in mind guys - the machines ONLY do what we tell them to do.

However, sometimes their creators put stupid little glitches into them - "rotten easter eggs" - to see if we're paying attention.

I contend that programmers who leave these easter eggs in the code are perverted SOB's with small you know what's and that's how they get back at people for being picked on when they were young.

That or they never worked in hard metal.

Still contend it is due to minuscule you know what's.

[MarshCustom]

I had another problem this week that resulted in srapping the part. I thought it was the same old cutter comp problem, but turned out to be a new problem. I was rough cutting a slot with a 1.25 shell mill when it tried to cut through the wall of the slot. I checked the tool path and all looked good. When I looked at the screen on the bridgeport I noticed the prev, current and next line of code. The current code was out of order. The machine had lost its place at picked out a random line. Replaced the part and hit Run and it cut perfect.

[NC Cams]

Marshcustom: The following assumes the use of a DX-32 PC or CIB DOS based computer in your Bridgeport.

The DX-32/DOS 6.22 based code was written BEFORE:
1. HDD's over 540K were made
2. LBA mode was incorportated into computer BIOS lexicons.

if you have installed a larger HDD with a conventional instead of a a 540K format or use LBA, the caching function of SMARTDRIV will put data into an area of the HDD of the machine but it WON't go back there to look for it - it can't because the software doesn't know larger HDD's ever existed.

We learned this the hard way on our Eztrak system with PC based DX-32 system. It got so bad that we couldn't even 'fix' the HDD.

We had to:
1. go into bios and turn OFF LBA mode
2. turn ON "write back to cache" before exiting
3. reformat the drive to 540K with FDISK.

These random glitches have disappeared after doing the above.

[manhasset]

:drowning: WE use FeatureCam for our CNC programming. Can someone tell me why every now and then the cutter path will stop and cut a perfect circle into the job (usally scrapping the piece)?? This only ever happens during the roughcut. WE have HAAS's, Bridgeports and JohnFords and this has happened on all of them at one time or another. The problem is that this circle cut does not show up when you view the cutterpath in FeatureCam but is obviously being posted out with it!!! The last time all we did was load the surfaces back in as iges instead of step and the circle cut went away???????

Any help would be greatly appreciated!!!

make sure you do not have on part line program found in the properties tap where you click cut comp. try it

[manhasset]

make sure you dont have on part line program located where the comp setting is . try it