Class "A" Surface Machining

[McRae]

Have you cut this yet?? Waiting for an update.

[Tri-Tech]

Not yet?

 

It will be a faw weeks before I get to it.

 

Regrads,

Ernie

[olib]

Tri-Tech

From memory and my experience modeling in 3D Studio Max, NURBS (Non-Uniform Rational B Sline)surfaces are described mathematicaly by spline curves. Take a any cross section of any NURBS surface, analyse it and it is always a spline. Refering to your old skool experience using splines in Mastercam version 3 or 4, sounds like NURBS is the way to go in combination with an "along" distance. I am only new to the whole CAD-CAM thing, but the hardest thing to get my head around is the fact that NURBS is not incorporated into everyday CAD-CAM. It is either arcs or straight lines.

[Guest CNC Apps Guy 1]

olib,

 

quote:

---

...but the hardest thing to get my head around is the fact that NURBS is not incorporated into everyday CAD-CAM...

---

There's only one problem with your position, not every CNC contol supports NURBS. As a matter of fact, if I had to make a semi educated guess, I'd have to say that roughly fewer than 25% of the contols on the market today (not to mention the dinosours out in shops right now) have that capability.

 

For Fanuc controls, you either have to have a 16MB or higher, or a 15MA or higher. That excludes a TON of controls out there. Siemans, Heidenhein(sp?), and Fidia offer it on their High End controls but the market presence of those 3 combined is probably only 30% of Fanuc's market share. It's not a very economical investment in time from a CAD/CAM Software Developers perspective IMHO, but just for the record, I wish that MC supported NURBS output as well, I think that market for that segemnt of machining will grow tremendously in the next 5 years as competition will drive companies to invest in better technology.

 

JM2C

[Lucky]

I received my Metacut Finish Pro software a few days ago. Very slick product but it appears it will do me no good. My Heidenhain TNC 430 control does spline interpolation but that is not the same as NURBS ( control points, knot weights, etc.) Metacut only supports Fanuc style NURBS. I do not know of a CAM system or 3rd party software that offers any support for Heidenhain spline interpolation.

 

CAM system support would be easier if all the control manufacturers would use Fanuc style NURBS as their standard.

 

Anyone using spline interpolation on their Heidenhain???

[CAMPOST]

Hi Lucky, I know that it´s too late, but you can use a dedicated post from ICAM to use arc-fit/nurbs-fitting feature in order to filter you toolpaths and get Spline Bezier interpolations used in Heidenhain controls.

 

Bye

[Guest CNC Apps Guy 1]

Boy, this was a LOOOOOOOON time ago.

 

I'm curious as to how/if the situation was resolved as I KNOW Ernie is a Fatal , errrr Fadal guy and that's all he's got. j/k Ernie.

[JG]

quote:

---

Filters remove points I need it to add points to the program.

---

quote:

---

The difference is, I had control over the along distance of the toolpath. Now it is controled by a curvature tolerance. This is where I think the problem is. If I had a option to use along distance instead of the curvature tolerance, I think the problem would go away.

---

Depending on the geometry, maybe 5ax multisurf with a locked vertical vector (3ax output) would help.(you can set the distance in both the along and across direction)

 

Thanks,

 

Jg

[Bill]

you know James, RandyN posted in this thread as well mentioning the facet problem, and at that time we (Randy and I) were using Fadals at Omega.

 

Sure was a long time ago. Three shops ago and I have had two different member names.

[RandyN]

And look at your post count, don't you ever work?

[smokey_44]

"Ever try machining like at 45 Deg. or 135 Deg? Lots of code but you'll get good results."

 

 

I do this everyday with 3d die forms and results are excellent

 

 

Dave

[Kelly Burns]

quote:

---

I do not use filters.

---

How can you not use any filters? And why would anyone be against using them anyhow.

 

We use them to make sure things remain "tight".

Also it aids the machine in cut transitions;

also it makes a cleaner program,less regen time

verify etc.

 

I dont understand the benefits of not using them.

 

[within a thou]

I think the form should dictate the angle used to cut. Why would you set a standard?

[Rick Henrickson The Boeing Co.]

I am not sure what a class "A" surface is?

32, 16, 8, how does it correspond?

[Guest CNC Apps Guy 1]

I think Ernie defined what a "Class A" Surface is earlier in the thread. This whole thread is a good read IMHO. Good information for surface machining.

[within a thou]

Another thing I have noticed is the smaller the rad on your cutter the better the finish. is there anyway you can go to a bull nose instead of a ball and use the ball only in areas needed to be?

[Bill]

"A" surface in the mold industry is a part that is something aesthetically pleasing. Interior trim that is visual always falls into this category. Usually requiring graining.

 

I still can't imagine cutting anything with NO benching afterwards unless they were looking for a certain pattern which he mentions.

 

I remember when I first got into this trade. We were building molds for name plates and gm I think it was wanted a spiral pattern like a record. (record for you young guys was vinyl and had grooves which produced music)

 

I dunno but back in '87 a few years before I got into cam, I had no idea on how to achieve that.

 

Guess I could tried it on a cross-slide.

 

cross-slide(another old machinist tool)

[Rick Henrickson The Boeing Co.]

This is a great thread, I will say that the machine tool you are using and its options will have much to do with surface ability! all machines are not created equal.

Okuma has one of the best surfacing options you can get, along with Makino, many of todays machine builders have gone to high speed and the ball screw pitch is large to make them faster.

I have done many demos on Okuma's with almost perfect surfaces but that is because it has all the options.

[billystein]

Quote

 

"In the old days using Mastercam Version 3 or 4, I did tooling for optical lens, machined aspheric surface shapes that where defind by mathematical equations. I would make a basic program to compute the points I needed to create splines. Then I would use the old toolpath stuff called Loft, select the splines and set the along distance to .02" or less. I would get a Class "A" surface."

 

 

Hi Buddy,

 

This may sound too easy but maybe you could try the loft toolpath again.It is still in version 9 somewhere.

 

 

P.S. Don't tell James that you want to run this on a Fadal

__________________________________________________

[Greg Williams]

quote:

---

but you can use a dedicated post from ICAM to use arc-fit/nurbs-fitting feature in order to filter you toolpaths and get Spline Bezier interpolations used in Heidenhain controls.

---

ICAM = BIG $$$$$$$$$$$$

 

I have had limited experience with ICAM, It semms to work very well and so it should for the big dollars

[cadcam]

billystein and couldnt we just use the scallop tool to get even better on say a Concave feature like this.

[gmenzies]

using filters

 

we started using metacut finish several years ago.

 

http://www.nwdesigns.com/Products/MCFinishNutshell.htm

 

I would recommend this product for anyone using a Hass or fadal .

 

the program uses the machine dynamics to filter the toolpath to achive maximum feed rates with out loosing accuracy and finish.

 

eg: surface finish contour with a cut tolarance of .0002 in mastercam.

 

mastercam posts out at six decimal places.

 

when runing the program through metacut finish.

the file is then reduces to 4 decimal places.

the file is processed at a tolarance of .0003

allowing arcs to be fitted.

g17 , g18 or g19 plane arcs are added

accell and decell are also added G8 and G9.

 

we cut alot of bottle molds and do hard milling.

we have found using swiss cutting tools for finishing benaficial ( DIXI or Fraza )

 

we try to rough down cavitys to have a constant

finish depth, usally .010 to .015 , stepover and cutter diameter all factor into the finish results for minimal polishing.

 

you may also have to look at you maching approach. possbly you may have to blend a couple differant tool paths to get the results you need.

 

as far as your iges data. crank up the shader in mastercam and look for anomolies in the surface.

rotated it around, we find alot of bad data this way before machinng.

 

try differant translators. we have alot of success with parasolid. step never seams to work

 

-- from my understanding of class A surface

is that you cannot feel the transition (Blend)

from one surface to another.

 

-- class B surface you cannot fell the transition

but you can feel the radius

 

-- class C -- normal fillet , where you can see and feel the transition.

 

surface finish is a hole differant ball game.

 

ie: number 1 finish is optical class. and on down from there.

 

Good Luck Ernie

 

Gord

[CAMPOST]

quote:

---

ICAM = BIG $$$$$$$$$$$$

 

I have had limited experience with ICAM, It semms to work very well and so it should for the big dollars

---

For sure. We are purchasing a seat of CATIA V5 here, and ICAM it´s the right post-processor for this software. But it´s really expensive, around US$ 10K for a dedicated license for our 10 DMU 70Evo.(Not the post builder license) It´s fair, if you want to enjoy all the features included on your control, and if you have complex parts to justify it. I know very well how the Mastercam MP language and its post processors works, and actually, ICAM post it´s not a interesting investment to use with Mastercam, because MC has in my opinion, the most powerfull post language among the CAM system around the world, the only thing that is missing at this moment is NURBS interpolation on Mastercam. CATIA for instance, it´s very burocratic, because depends on the APT and PPTables, that for me, just complicate the things. You can´t have got the codes and the post logic with the same flexibility thats MC allows. Well, you can,but it´s much more complicated, and normally you depends on third suppliers in order to do it. But if you really want to have Bezier interpolation on your machines using Mastercam, at this moment, ICAM it´s a good option. Does anybody here knows if CNC software intends to implement NURBS interpolation on Mastercam?

 

Thus

 

And sorry for my wrong english.

[Guest CNC Apps Guy 1]

I've been asking since like 1998. Guess there is really not that much of a demand.