Need some advice:

[clayman]

does anyone know what program i need to put my autodesk (Inventor) drawings into a Fanuc o-t controller? i'm new at this CNC thing and I had an Engineer tell me that this controller could read my 3-D drawings with the right software. is this true????????????

[g-codeguy]

Don't think your engineer is right. OT controls run on G-codes as far as I know. We use Mastercam to get the G-code. I don't use Inventor, but I did watch the guy who does move the file from Inventor directly into Mastercam. You then need to define the operations, and run them through a post processor made for your specific machine, not just for an OT control.

Reason being machine builders have their own thoughts on what codes to use. Hardinge uses an M13 to turn the spindle on with coolant. Mori Seiki uses M3 to start the spindle, and requires an M8 to turn on the coolant.

Hardinge has what they call "Blue Print Programming". We have machines with this capability, but have never used it as our programs all have to be easily modified to run on other lathes. Don't know how it works, but doubt you can read an Inventor file into the control.

I'd be interested in what you ultimately find out. I've been wrong before.

[clayman]

Thanks, Something told me that it couldn't be that easy. I was just looking for an easy way out. The G-Code thing is great but the problem is I have been manually machining for 24 years and this programing stuff really freaks me out. The guy that had this machine passed away so i've been filling my coordinates into his programs. This controller will not let me write a new program. I turn the dial to Edit and hit program but it just goes back to the last one that ran. I realize that this sounds STUPID but i have no manual and i'm trying to figure this from scratch. Can anyone out there tell me how to clear my screen and start a new program????

Thanks,

[cam1]

Hi: You are on the vertical potion of the learning curve. Pickup a basic CNC handbook (Peter Smid), and get the basics. Short of that, even with your manual machining skills, there is a very high probability that you will damage the machine, or worse, hurt yourself.
The fact that it freaks you out, tells me that you are nervous or uncomfortable with this, so build some confidence the safe way, get some demo software, have the re-seller give you 1 hour of the basics, and hit the books...

regards

[Andre' B]

Learning to run and program a CNC is very hard to do if you do not have someone at hand you can ask questions, without proper documentation for the machine it will be all but impossible.

Get a set of manuals, ebay, call the guy you deal with for repairs he may know were to get some cheap, or get new set from the machine builder. If nothing else get the manuals for the control from Fanuc it will not cover anything the machine builder modified but will at least cover the control.

Whatever they cost will be less the time you waste by guessing how things are supposed to work.

Smid's books are very good, frequently easier to read then the machine manuals.

If you want to practice programming look into a simulator, where crashes just mess up the computer screen. It will not do everything exactly like the machine but if it works on the sim you are that much closer to a running program on the machine.
Here is the one I use the most.
http://www.ncplot.com/

[g-codeguy]

Clayman. What machine are you trying to program? Can't be of much help not knowing that.

A couple things: First there is an Edit key. Is it turned on so you can edit? Second thing: To start a new program type in the letter 'O' and the program number. (up to 4 digits.) Do not use the EOB key yet. Hit the INSERT key. Not literally of course! No matter how frustrated you might be. Now you can use the EOB key to separate the program number from the next block. OT controls allow only one word address to be entered at a time. Programming on the machine is very time consuming to start with. One word at a time makes it worse.

Another thing you can check before starting is to make sure you have enough memory left to add more programs. While in EDIT mode hit the "Prog" key to make the directory come up. Available memory space and number of programs available will be on the upper right.

I know you have been machining for years, but I haven't a clue as to how much you know so I apologize if most of this seems to question your intelligence. It isn't meant that way. Just trying to help you get started.

Remember...the programming manual that came with the machine is your best friend. It will tell you what all the programming codes mean and how to use them. Some manuals even explain how to use tool compensation. You have to know how to figure tool compensation in order to program the tool correctly. This requires knowing how to figure trig for right triangles.

If you know how to use G41/G42 commands then you don't have to worry about figuring tool compensation. However, using these codes has there own idiosyncrasies. You have to put the tool nose radius in the Geometry page. You also have to input the tool nose position (1 thru 9) in the tool geometry page. I can't help you there as we don't use these codes in our shop so I never learned how. I do know that it requires starting far enough away from the part to make a move for the tool compensation offset to take affect. Not sure that I am even explaining this correctly.

Good luck getting started. Programming isn't hard. Since you have been machining for years you should already know how to best program the operations.

EDIT: Well programming isn't hard if you are doing it for a lathe. 4-5 axis mills are another story. Programming a lathe for C-axis or Y-axis isn't too easy either. However you won't have that problem on a lathe with an OT control. You won't have these options!

[clayman]

Thanks everyone: Especially (G-Code Guy) Sorry i took so long to reply but i've been reading and programming! Everything is going great Turning Drilling Boring Etc. However, I am having some problems with the G76 Fanuc threading cycle. The manual seems like it was written in another language and then translated. The G76 has two lines. in the first line I am Totally lost. G76P (m) (r) (a) Q ____ R____; The next line makes perfect sense for a Machinist with thread depth,X and Y Etc. I'm guessing that this is probably very simple with the right Instruction?????? If anyone could help with this I would be greatfully appreciative.

Thanks again, clayman

[g-codeguy]

Originally Posted by clayman Thanks everyone: Especially (G-Code Guy) Sorry i took so long to reply but i've been reading and programming! Everything is going great Turning Drilling Boring Etc. However, I am having some problems with the G76 Fanuc threading cycle. The manual seems like it was written in another language and then translated. The G76 has two lines. in the first line I am Totally lost. G76P (m) (r) (a) Q ____ R____; The next line makes perfect sense for a Machinist with thread depth,X and Y Etc. I'm guessing that this is probably very simple with the right Instruction?????? If anyone could help with this I would be greatfully appreciative. Thanks again, clayman

Bummer. Was halfway thru my reply when the computer shut off. Wasn't a power problem as I use an APC. Will try again.

You need a Hardinge manual. I'm not at work, but I think I can remember how it all works. (m) is the number of times the tool repeats after reaching the root diameter. These are called 'spring passes'. A value of 03 would have the tool making 3 spring passes. Usually not a good thing on work-hardening materials. It can help remove thread taper caused by the part pushing away from the tool.

(r) determines how fast the tool will retract at the end of the thread. I believe this number is a multiple of .1 and is multiplied times the programmed lead. 00 means the tool doesn't withdraw until after reaching the final position. Normally I will use 00 only when there is a thread relief as it will leave a ring on the last thread. I program 01 otherwise as I want the tool to retract over the shortest distance. On a 1/4-20 UN thread this would cause the tool to retract at .1 * .05. A value of 02 would be .2 * .05, a value of 14 would be 1.4 * .05, etc.

Be aware that spindle speed will also affect how fast the tool will retract even tho the value is the same. Often I am threading to a shoulder and have to be within a certain distance. Slower RPM will allow the tool to stay down longer for any given (r) value. This can determine the grade of insert you need for the job. Not all grades can handle running way below their intended SFM range.

I have found that dropping below S900 has no affect. We have one job with an internal thread and a face groove at the thread diameter. There is a seat on the shoulder face below that (in X-diameter). I can't get close enough even at S900. Have to grind relief in the side of the insert to attain thread depth. Sandvik has the only insert grade of those we tested that will last at that slow SFM.

(a) is the compound infeed. You have 6 choices on the G76 2-block call. Control divides this number by two to determine the compound infeed. 00 has no infeed in Z-axis. I would stay away from 00 as this creates the toughest chip. I use 60 only when trying to eliminate chatter. This has the least amount of tool pressure, but the insert is rubbing on the back side. Not good in work-hardening materials. Not too good if the machine has excessive backlash and has a hard time repeating exactly on Z-axis as the back side of the thread might not be smooth. I usually stick with 29 or 55 degrees for 14.5 or 27.5 degree compound infeed (respectively)

Q is the minimum amount per side (until the last pass) that you want removed per pass. Q30 is my standard value...normally. In such materials as 316 SS you want to keep the insert below any work-hardening from the previous pass. That is why

R can be used to specify the amount (per side) of the last pass. DOC for the last pass would be .0005 per side for a value of R.0005.

Hope this has been of some help to you.

[clayman]

Thanks again G-Codeguy! This was more helpfull than any book i've been into so far. I'll for sure be threading on Monday morning. Hopefully, someday I can return the help.

Thanks again to everyone for the advice. I tried jumping into this way to fast. Now realizing that I must take the time to read and learn. These machines just move way to fast to be making errors!

[g-codeguy]

Originally Posted by clayman These machines just move way to fast to be making errors!

Try using the Rapid and Feed-override controls. I hope you are testing out new programs by cutting air the first time thru. I prefer to run them thru with the rapid all the way down (when turret is close to the chuck). Then run them thru again with the rapid all the way up. First time thru shows any obvious errors that could destroy a tool. Second time thru will show me if I missed a G1 which could break an insert (and possibly destroy the tool). Rapid on lowest setting is slower than some feedrates.

I just had an operator destroy the pocket on a 3/4 in. groove bar because I had typed in X2.94 instead of X1.94. Had he tested the program out first, he would have seen the error. Always provided he could figure out that an ID groove bar that was going higher than the OD of the raw material was a problem!

Most guys in the shop have become too trusting of my programs, and don't test them before cutting chips. Guess what. I'm not perfect. One more reason for using a CAD/CAM program. It doesn't make typing errors, & the one we use will let you know if there is an interference problem with the tool. Like trying to run a 1/2 inch boring bar in a 3/8 inch hole.

[clayman]

Hi: It's been a while but haven't had much work for the CNC lathe It's been alot of oilfield repair.(manual) Just wondering if anyone could tell me where i can get my hands on a Hardinge manual as (G-codeguy) had suggested. I tried online but all I could find were used hardinge machines for sale. I have some 4 1/2 EUE casing threads to do. 400 of them. Still haven't threaded to much on this machine and the manual that came with it is a translated chinese version that is incredibly hard to understand. If anyone knows of some decent books that would help me with a Kingston lathe that has a FANUC series 0 controller I would greatly appreciate the help.

Thanks fer now, clayman

[stuby]

I have a Leadwell LTC-15 2 axis lathe with a Fanuc-OT controller on it. I found my operators manual, which has basically everything in it, on ebay. They come and go. I am a self taught G-coder, and I have no software either. And trust me when I say this : The operators manual is like your bible. I noticed with my OT controller it likes the canned cycles in 2 seperate lines, not sure why; Anyways look for that on ebay, if you have no luck, send me a msg, I can photocopy some pages of threading codes for you if you need.