What's new
What's new

looking for offline software for Faunc 16W controller

tlmkr38

Aluminum
Joined
Sep 27, 2008
Location
Dresden, Tn
We just bought an older Fanuc Robocut with a 16W controller. This is our first EDM and we just need it for small die repair and stuff right now. I would like to be able to program it offline but it didn't come with offline software. Is there any available or do I need to look into 3rd party software? If 3rd party what is a decent inexpensive one?

Thanks!
 
Hi tlmkr38:
Assuming your machine eats G code like every other Fanuc machine in creation, you have a huge variety of choices that will work.
All you need is a post processor that will speak "Fanuc".

I run an old old version of Mastercam Mill (version 8.1 not X8!!) and just call my cutter 0.010" diameter.
A buddy of mine runs Bobcad and says it works fine for him too.
Another buddy swears by Esprit, but he pays a LOT for the bragging rights and I don't think his parts are any more complicated than mine.

Programming on a wire is not very demanding; it's setting up and processing strategy that is the big differentiator in wire work.
Wire work is typically super accurate work and the gremlins that give you the ass bite are not usually the toolpaths...it''s the operations order and the stock allowance and the fixturing, and the stress release and the overcut allowance and the flushing and etc etc etc.

If you're already into CNC milling, I'd first see if my milling CAM solution could be made to work.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Implex has it right on. Writing the code is the easy part. I would suggest write some real simple programs run them in dry run see how it moves. Then get some scrap put on your patience cap and try cutting. Guarantee you will run into problems you have no idea how to fix. For example, wire breaks but why? Wrong settings, bad water etc. even if you have manuals probably no help there.
Bob
 
I use Cam-i and it’s quite amazing software. Just draw your part, pick your path and away you go! It’s the easiest software I have ever used for Wire EDM.
There is a heavy cost of about $7000 for it initially but there is no yearly maintenance fees and it has every machine Fanuc build in the programming.
I have three different wires I run and by picking the proper machine, all the tech is right there. Even taper cutting is quite easy.
 
All I have right now as for a 3rd party program is one called CamBam. It's inexpensive but it pretty good for what we do. I can see how programming the G code with it would work good with that on a straight cut. HOw can you use it to program like die clearance angles and stuff?
 
Hi again tlmkr38:
My experience with different brands of EDM machines is not very wide, but on all I have run, the most common command to run a simple non-varying taper is created by inserting a taper command word into the beginning of the code string and a taper cancel word into the end of the code string.
On my Chmer machine which will run from the code created by a standard Fanuc post, the command to begin the taper is "A" followed by the taper angle desired (positive or negative value depending on whether you want the big end at the top or bottom of the part.
Taper cancel is "A0".
Every different machine brand seems to use its own unique word, so "A" may or may not work on your Fanuc.

For the majority of taper work on punch dies this is how it's done by pretty much every machine I've seen code for.
There is another way however, and that is to write the code for the upper profile, write the code for the lower profile and stitch them together line by line.
This is called "Complex Upper And Lower" programming (by Sodick which was the machine on which I first learned it) and is used when the taper varies as you go around the profile.
I am not sure if every wire machine out there can do this but I see it relatively rarely in sample code so I suspect not.

In addition to the code, you also have to set up the machine, and this is typically done on some kind of taper setting screen in the control.

Using my Chmer again as an example, I have a taper set screen in which I can input first of all that there will be a taper, and what it's angle will be.
Then I can tell it how I want to instruct the machine, whether to use the "A" word, Complex Upper and Lower, or command the U and V axes directly.
Last I can tell it how far above the platen surface I want the taper to begin...you would think of this height as the die land height if you're making punch dies.

All of these commands are simple inputs and I believe all wires capable of cutting tapers will have a screen like this.

On my machine it is also possible to input much of this by writing it into the code instead of commanding it from the screen, but your machine may or may not be able to do this.

So that's really it: sounds terribly complicated but it's actually not too bad once you figure it out the first time.

For your stated purposes, you will likely stick to the simplest way which is to manually insert the taper commands into the G code your CAM system has spit out, find and edit the values on the taper command screen, simulate the code to be sure you commanded the taper in the proper direction (Big on top or small on top as you prefer for each job), and push the big green button.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Thanks for that info. Once we get it in the room and hooked up I'm sure I'll find more of this stuff. I have all the books with the machine and it tells about how to do the manual programming and all as well as like canned cycles. Like you say once I get to using it and do more with the machine it will get easier. :)
 
Yep it took about 3 yrs to finally get the machine in the room and running, long story... Thanks to some folks on here I have gotten it running and have made some straight cuts and figured out offsets and all as far as how to lead into them. Still working on settings and what works best for efficiency but I'll get it. Tried some taper cutting the other day and it didn't quite work like it should have or like I thought it should. Just came back to this post nd saw what you had written about Using the A word for setting taper. This machine uses T I believe and I'm gonna try it in the morning and see how it works. Have a die modification job coming up that I need to use the taper for relief for the slugs on the bottom. Hopefully it will work. And your right, all of this looke complicated as heck until you figure it out then it's pretty simple.

Thanks!
 








 
Back
Top