3D milling problems with fanuc om

[Anonymous]

So I have a question for you guys I have been machining with my CnC for 6 months. So I'm very green lol. I have a 96 kitamura mycenter 1 with a fanuc OM controller. So when I'm machining 2-D Parts. It's works Great with very few hiccups. But when I'm trying to do longer programs Or 3-D milling it starts at locking up in the middle of the program Sometimes if I just go back into Fusion 360 and just post where it locked up instead of the whole job it will work. Other times it will work flawlessly till the end and with 10% left of the code it will lock up and I will get a drip feeding air on my control. Which does not happen on 2d milling normally. I was wondering if there's anybody that runs a OM controller. That could help me out Either contact me on here or email me at Backfirefab@gmail.com
Thank you
James

[Steinwerks]

What's your baud rate for drip feeding set to?

[Anonymous]

4600. My machine says he can do 9600 But when I try to use 9600 ( even with the parameters set for 9600 on the controller ) it it does not work at all

[Anonymous]

Any help would be greatly appreciated

[Laurens-3DTechDraw]

How long is your cable for the drip feeding?

[Anonymous]

Between 8 and 10 feet With a USB to serial adapter

[Anonymous]

I would try running it of a computer with a true serial port. Sometime when you add an adapter with its own chipset it can cause problems. Or Highland Dnc make a decent product from what I am told.

[Steinwerks]

I also would recommend trying a computer with a serial port directly if you can find one. A lot of workstation PC's still have them for backwards compatibility. I don't think I'd want to try DNC with HSM's code over anything slower than 9600.

I presume your machine has something like 64k of memory then? Do you have a PCMCIA slot?

[Anonymous]

So I switched over to a desktop that had a direct serial port. Ran a program and the same problem. In the same spot. How can I tell if I'm sending HSM code in my program with Fusion 360. I'm at the point where I don't know what to do. As far as memory I was told that this machine does it weird and that it's memory By character. And it says that there is 15610 free

Thank you for any help
James @ backfire fab

[Steinwerks]

Honestly I am not going to be a lot of help in this regard, we don't DNC anything, and I am far from a Fanuc guru. What I would suggest is signing up over at Practical Machinist and posting here regarding the issue: http://www.practicalmachinist.com/vb/cnc-machining/

Hopefully Bill Angel (angelw) will pick up on your post, the guy is practically an encyclopedia of Fanuc, and there are a lot of other folks over there who really know their controls inside and out. Be forewarned, it helps to have thick skin sometime too, but as you're not running a hobby machine I don't think anyone will complain.

Include as much information as possible in your initial post.

[Anonymous]

James, Lets take it back a step or two, 1)The program up until this point drip feeds ok? 2)Is this the first chunk of 3D type code? 3) Did you turn on smoothing for that operation before you posted? 4) have you tried another serial cable? 5) Can you upload the file you are working from or the code it produced? I suspect that smoothing was off and it it choking on whole bunch of small moves. You could try turning the feed way down on that section of code to see what happens. Sometimes if the control cant keep up it stops, if you have many small lines that only move .001 to .010 especially in all three axis this may be the case.

[Anonymous]

@Steinwerks I posted on practical machinist And not a single answer.

@Anonymous To answer your questions I'll start five beginning. I am using the fanuc generic post processor on a OM. So when I post a program this is the frequency of my machine running through the program
Drilling works 100% of the time
2d Contor 85% of the time
Chamfer 100% of the time
Facing 100%
Any adaptive strategy 30%.

So yes this is the first real 3D piece that I'm trying to make with contours. I am running the smoothing on it is normally set to .0004 for me. Today I was trying different things And moved it up to .001 and .003 which made it worse and lock up sooner. Today I also tried cutting the speeds and feeds and a half So on my 3-D contour I was using a .500 ball mill running 10000rpm @ 60 imp with a .003 chip per tooth. I reposted it running 6500 rpm @35imp with Close to the same chip per tooth. And it locked up about the same time that it always does in the program 20%-30%. I also went to the settings on both my laptop and the desktop and set the serial cable outputs to match my Machines compatibility. I have not tried a Nother serial cable but I bought this one specifically from a reputable Cnc company that was designed for a fanuc. Which at this point I don't even know if that's true Lol.
As far as posting the code how do you want me to do it do you want me to just copy and paste the whole file up ??

Thank you for your help. At this point I'm almost ready to sell the machine. I've had a CNC programmer come down that couldn't help me out I had a CNC mechanic come down that said I needed to talk to a programmer . I'm just running out of money and I may have jumped into deep Lol i'm at the point where I may have to cut my losses The program that I'm trying to run right now it's supposed to be 4 1/2 hours long And I am in it for about 12 hours of starts and stops Right now and I'm not even half done

Thanks again
James moran
Backfirefab@gmail.com

[Anonymous]

a part of my post

[Anonymous]

This is probably a little more technical than you want or have the skills for but I am not sure where you are with getting into it at this level so I apologise if you already know this?

RS232 has a number of issues transferring data where the end device does not use handshaking or is not correctly wired for it. Basically, this means that the end device can tell the sender to stop sending data as the buffer is nearly full and will restart this when it has enough space to handle more.

In the cable, you have 3 wires, transmit, receive and ground. These are the minimum required for data transmission and often referred to as a NULL MODEM connection. There are 2 ways to do the handshaking, software and hardware. Software is ideal when you have only this 3 wire connection and does this by sending certain bytes in the telemetry. Not so common these days. The second method uses 2 additional wires in your cable, referred to as RTS (Ready to send) and CTS (Clear to send). RTS is sent from the sending device to indicate it can received data and CTS from the receiving device. If the CTS is not active, the sending device will wait until it goes active.

Are you able to open up your cable connectors (normally just a couple of screws or a latch type) and check what wires are connected. The PC end should normally be a 9 pin D-type and the pins are numbered on the connector? I can then work out if this has hardware or software handshaking. Also check if the software itself has any options for setting hardware handshaking.

[Anonymous]

Thank you I'll open the cable and take some pics on Monday morning

[randyT9V9C · Accepted solution]

The 0M control has a fairly low block number limit. When you hit the limit the error it generates is rather vague. Turn off block numbers in your post, showsequencenumbers=off, on the post dialog. That should fix your stopping on large files.

To use 9600 baud you have to set the baud rate in both the CNC side and the the PMC side. Toggle the CNC/PMC (NC/PC) button and it is on one of the screens in the PMC, The setting on the CNC side sets the i/o parameters for the serial port that hooks to your computer. The PMC setting sets the internal speed (baud rate) between the CNC and PMC. I bumped mine up and DNC at 9600, although I can't say it huge difference.

I did install a Calmotion USB interface on the machine about two years ago and it works great. Nice having a 1990 vintage machine with a USB port. 

http://www.calmotion.com/usbcnc-int.html

[Anonymous]

Hey I just want to thank everyone on here that helped out. Today was the first time I actually ran a 3 1/2 hour program flawlesslY. And all I did was check a "no" in the post processing Lol thank you Randy for the simple fix. I was pulling my hair out.