Help 3D mazak gurus!

[Freddy]

We have a simple 2" radius semi circle with 1/8 radii on the top surface. When we machine this on our Mazak VTC30 M+ using a 3/4 ball endmill, the cut starts on the top. It then travels around the 1/8 radii down through the 2" radius. It starts up the other side removing material. It gets to the top of the other side around the 1/8 radius. The cutter then moves over .005 to repeat the process from the opposite side. Only this time it starts down, but moves away from the material. When it gets to the bottom of the 2 " radii, on its way up it starts to cut again. It only cuts on its way up. Mazak applications and Mastercam applications are scratching there heads. We contacted both to try to figure out our problem.

Mastercam applications actually wrote the program. So this eliminates us as the problem.

This is suppose to be simple stuff, I thought.

Anybody have any ideas? Mazak or Mastercam? Post or Communications?

[BernieT]

Any chance you could put it on Cadcam's FTP site so we could look at it????

 

BerTau

[Freddy]

Freddy.nc in the NC files folder.

 

I also have a .mov file viewable with quicktime, but its 20 meg. If it can be of some help, let me know where to put it.

 

Thanks,

Freddy

[BernieT]

quote:

---

Freddy.nc in the NC files folder

---

I would need the .MC8 file to be any help. Sorry.

[P_Scott]

Freddy,

 

Welcome to the Forum. What version of Mastercam are you using? It usually helps to include the Mastercam model file (.mcX) to provide more specific information to those who may be able to help you. If it is too large to e-mail to anyone, perhaps you could download the Mastercam file to the FTP as you did with the .NC. I've checked the file in Cimco Edit V4 with the Backplot and the .NC program appears to be a normal Parallel surface toolpath. What are the parameters for the operation? The best way to look these things over is from the Mastercam file directly. Have you contacted your Mastercam reseller for tech support? Go to this website Reseller Locator if you need help in finding your local reseller. HTH

[Allan]

What is the feed rate? try going sloooow see if it cuts. Sounds like the machine is not tracking arcs correctly. You could shut the filter off in MC.

 

HTH

 

Allan

 

Ok looks like it is 15IPM, and linerized code. Try arc filtering and tighten up the cut tolerance.

 

[ 05-20-2002, 03:45 PM: Message edited by: Allan ]

[Freddy]

Looks like Mazak solved our problem. I won't know for sure for a couple of days, but things look good.

 

They had us add a g61.1 at the beginning of the program. From what I understand, it stops to check data?

 

Anybody care to elaborate on this? I know just enough to be dangerous. I'm sure it will help other Mazak users.

 

Anyway, thanks for a great forum. I think I'll start hangin' around here.

[PE @ IHS]

The G61.1 code for Mazak controls is a modal version of the G09 Exact Stop command (one shot code)

 

Essentially, these commands are used to decelarate the tool at the endpoint of each interpolated function (G01-G03) and check for in-position status. The CNC checks for the correct position before continuing.

 

To put it simply, this code is designed to eliminate overshoot of your axes.

aka Exact Stop Check Mode on Fanuc controls

 

Peter Eigler

[Scott Bond]

quote:

---

The G61.1 code for Mazak controls is a modal version of the G09 Exact Stop command (one shot code)

---

Good Morning all

I have a Fanuc 16i on our OKK Horzontal.

What would be the best way to get the g09's

only where I need them, on outside corners ?

[Mike Whitten CAD/CAM Contractors]

Scott,

 

I am not exactly sure how to answer that but it would seem like a post issue.

 

I would like to add this though. I have ran Makino and Matsuura late model (5-10yrs) Horizontal machines with Fanuc 16 controls. all of these machines had a Look ahead Function. This was a G08. This Function completely takes care of servo Lag and makes programming much easier. You may want to verify that you do not have this Function. If you do, you are all set.

 

Mike

[crazy^millman]

Our Fadal machines have this type of a function and it is G8 i have our post hard coded to use the G8 all of the time. It is rare we are not cutting 3d work so best to have that default all the time.

 

HTH

[Mike Whitten CAD/CAM Contractors]

Millman,

 

I am not a Fadal expert but I just am wondering why you have to run a G8 on a Fadal?

 

Are you running Format 1? I think that if you run Format 2 this is not needed

 

Mike

[Mike Whitten CAD/CAM Contractors]

Millman,

 

I worked at a place once where we did nothing but sculptured surfaces on Fadals. At the time I was not programming this stuff because it was all done in Pro-manufacturing. Anyhow, what we used alot was M94,s. Pro-E has some very nice 3d paths that actually look like a Parallel cut but are actually calulating scallop height in the across direction. I noticed that Merlin was talking about this a few months back. Anyhow I believe that the M94 limits the Servo Lag when the Axis changes by a specified angle. It is in the book. This Function would work well with Flowline and Parallel Toolpaths.

 

Have you used this?

 

Thanks,

 

Mike

[crazy^millman]

Taken from Fadal's website:

quote:

---

This code is used when no hesitation is desired between moves. If the tool

hesitates the tool pressure lessens and the tool will leave a tool mark on the

contour. The G8 code would be used to eliminate the tool marks.

The hesitation is called a feed ramp or acceleration-deceleration. Ramping is

used to help the tool move to the desired position. • The G8 code is often used in combination with the M92 code.

• This code is modal and will remain in effect until the G9 code is used.

• The G8 code is a default code for format two.

• The G8 code is incompatible with a G41 or G42 coded on the same line.

• The G9 code is used to cancel the G8 code.

EXAMPLE: G0 G8 G90 (Ramping is off at this line).

G2 I.5 G91 Z.02 L7

X-.5 G41

X.55 Y-.55 I.55 G3

• The M95 code is used as a non modal form of the G9 code. It is generally

used when G8 is in effect. See M95 for more details.

---

As you can see it is a defualt code for 2 but if we do not have this in our post the machines act like G9 but if we have G8 in our post the machines work like G8. They are all in Format 2 but act this way. I look at it this way if it works and does the job the way we want it to then I am going to go with what works. I have even checked to make sure we do not get the M95 in our posts.

 

HTET

[Mike Whitten CAD/CAM Contractors]

OK,

 

I got it now.

 

It must be some type of config thing.

 

Thanks,

 

Mike

[Jack Mitchell]

Freddy,

 

Welcome to the forum.

 

If I were to attempt surfacing a miniature staircase, up then down with .005” radii at the corners of each step – it would not be reasonable for me to expect a smooth finish at 150 inches per minute without the use of exact stop checking.

Your eyes tell the tale once you make this adjustment and realize that you’re not really holding 150 inches per minute throughout the entire path.

 

Try checking your parameter manual for this setting if possible – the way that I see it is that this would be the most beneficial solution when surfacing with tight break radii.

I have also encountered this problem in the past as many others here do as well.

 

My question back to the forum is this:

Is there some method of adjusting the feed rate to say 5% of the programmed rate at specific walls and corner breaks?

And if so, then would this not be a more preferable solution since it gives the programmer the ability to control the variables as opposed to utilizing the exact stop command though a programming control feature?

 

Great question anyways.

 

 

P.S. Looks sort of busy on the forum this morning at 2:00AM in Ontario (my time)

 

Regards, Jack

[Mike Whitten CAD/CAM Contractors]

Try "High Feed". I just tried a couple of small tests with sculptured surfaces and it seems to work. I used to use Metacut utilities(Northwood Designs) for this back about 5yrs ago. It worked great but Highfeed may also do it?

 

Thanks

 

From Help:

------------------------------

Intended use

 

¨ Works with 2.5-axis and 3-axis toolpaths.

 

¨ Applies only to machine moves specified by G0 – G3 codes

 

¨ Works with flat, bull, and ball cutters.

 

¨ All selected operations must use the same tool plane.

 

¨ Does not work with 5-axis toolpaths.

 

¨ Does not modify feed rates when cutter compensation in control is used.

 

¨ Does not handle position codes.

 

If the control can accept arcs, you can filter the operation prior to optimizing it with Highfeed (NC Utilities, Filter).

----------------------------

 

Mike

[steve f]

Yup, high feed is the way to go. The great thing about high feed is it incorporates feed modification based on material volume as well as the dynamics of the machine. If you're generating a finishing toolpath where only .01" of material is being removed than the only thing that will affect feed modification are the machine limitations (acc-dec, up and down feed, etc.). It also generates fast feed rates where no material is being cut saving time in the process.

 

A great but underused tool IMO.

 

steve

[Mike Whitten CAD/CAM Contractors]

So it even works good in 3D milling?

[Jack Mitchell]

steve,

 

quote:

---

A great but underused tool IMO.

---

Well said - I will try this in the future.

 

Regards, Jack

[iowajim62]

Freddy,

u said,

quote:

---

They had us add a g61.1 at the beginning of the program. From what I understand, it stops to check data?

---

This code is an error correction code from your Mazak manual to make sure the machine doesn't overshoot position. Very awesome arc correction at 600 ipm.

[Slixmix]

According to my buddy Rick McAllister, you can add a "K" value to your G61.1 to tighten up the tolerance. I believe it looks like this: G61.1,K80 The higher the #, the tighter the tolerance for holes, etc.. that need to be more accurate. I also believe the machine defaults to K70 if you don't put in a "K" value at all. Anyone else play with this value?

 

[ 06-02-2004, 11:34 AM: Message edited by: N FRANCO ]

[Scott Bond]

Good Morning

Thanks for the responces.

I put a "G8P1" at the start of each tool,

and "G8P0" at the end of each tool the was

not a drill (or equil to). ,, still have a little radii at 200IPM but it is a good fast part.

[Mike Whitten CAD/CAM Contractors]

That is exactly what we do on our Matsuura production machines.

 

Just set up the post to use a Mi and make it default to yes. That way it will always be on unless you turn it off.

 

Mike