Class "A" Surface Machining

[Guest CNC Apps Guy 1]

Your point is clear to me. The large curvature stuff often shows up for a few reasons, sometimes just one factor, and sometime a combination of them all. If the small stuff is showing up OK, and the large stuff is where the problem lies, then often the resolution on the servo encoder coupled with ballscrew pitch cannot make that small of a move in say z across that large of a move in say X. You say you're sure its not a machine problem but how do you know? Try putting say a 200" radius across say a 10" ling part. See what that curvature looks like. I'd almost be willing to bet money that there would be a fair amount of faceting. Having worked for a machine tool builder, I know Machine Tools, various cunstruction methods, and their limitations and this in one of them. You can only get so fine in resolution before you start to see the ballscrew pitch in your part, like it or not, it's just a mechanical fact.

 

JMNSHO

[Robby GM]

line between to points on a surface is control

under MC config tolerances /

Maximum surface deviation

i use a setting of .0002 mm

[Robby GM]

James is right. some machines just work better then other doing large 3d surface work

plus sometimes cnc controlers have acc/dec built into , i turn off all acc/dec.

with it on leaves a mark at end of each block of code

[pactec]

Hello There...

 

Let me chime in here. Since tensions are fraying, I would suggest a step back to analyze the situation. I strongly recomend filtering, not the way you think but look into the Northwood filter way of doing things. I have heard nothing but good things about it.

The second thing is to run one toolpath perpendicular to another and see if that removes the facets.

If you do a cut and some surfaces are smooth and some others are not then you have to look at the surface data. This makes sence since you take more than one pass on any surface.

Did you try different machining strategies to see if you could pinpoint the problem?

The verify in Mastercam may be slow, depending on your particular box, but you will see scallops and surface finishes. Again, Northwood does a nice job of verifying toolpath if you need that much more control.

Hope this helps and get your dealer out to your shop so that someone else can see what's going on. A picture is worth a thousand words.

 

Take care...

[Scott Bond]

quote:

---

I know it's a hard thing to do with Mastercam because you end up with facets or line patterns that are hard to polish out.

 

---

I can cut your file with Mastercam, with one try, and no hand blending.

So post it,( on CAD CAM's ftp)

I'll be glad to make your part .

 

quote:

---

I refer to a class "A" surface as one that is optically smooth. Any tips would be appreciated.

---

In manufacturing I refer to this as the "Cosmetic Surface"

 

[ 10-08-2002, 02:58 PM: Message edited by: Scott Bond ]

[STEELTHOM62]

Since we got our seat of MC 4 yrs ago, we've returned our investment several times over,however, the one part that we actually had in mind(a flow cavity for rubber extrusion that 'ramps' up from a 2" depth to a 1/2" depth, part of the way on a radius and the rest of the way straight),we've only been able to cut with straight lines.I've been told that not even Metacut will create the helical toolpath required to cut this.The polishing required to get these lines out by hand is minimal, though.

[Guest CNC Apps Guy 1]

quote:

---

This is for advanced users only, please.

---

I started thinking about this statement. It must be cool to be you. Knowing everything and all. It must be tough though, since you have no peers to ask information from, I mean sheesh, how could somebody that's not an "Advanced User" have anything positive to say? You could always call your reseller and perhaps the professionls there could offer up some advice for your dilemma?

[pactec]

There you go. You aren't going to get rid of scallops but you will get a part that needs minimal polishing.

This is a cosmetic thing and as long as the cut is tolleranced enough you'll get that.

I'm also wondering if when you import files if the settings under screen, configure, surface and curve deviation have anything to do with it, since Iges is a translator rather than a reader.

Tight tollerance, small stepover, and sound machining strategy are the ticket.

 

Later...

[pactec]

Put my message before James's last one. He was quicker than me because I use hunt and peck when I'm typing.

 

[iowajim62]

Hi Ernie,

You could turn the machine over to MM from

inches and that might help tighten up things

since it would resolve a little closer or is

that not possible with your machine?

Jim

[Tri-Tech]

James,

quote:

---

This is for advanced users only, please.

---

I meant users that have experienced cutting Class "A" surfaces for car body tooling.

 

Please do not take offense, I I'm not mad and I do appreciate all your inputs I just have a hard time explaining myself.

 

Thank you

Ernie

[Guest CNC Apps Guy 1]

OK Ernie,

 

But, try cutting a very large radius (similar in size to the raduis you're trying to cut on the Class A Surface) on a small block of something. Just a simple contour. This will give you an indication of what your machine is capable of resolving, and will show you the results you should reasonably be able to obtain on your machine. A simple contour tells a lot.

[Greg Williams]

Mr Tri-Tech,

 

To be humble is to be brilliant.

[Trevor Bailey]

james is correct. if you are not willing to look at the source of the problem, the cad file, then you need to use his "cut test". this will prove everything needed for future jobs/knowledge.

 

good luck,

[Jack Mitchell]

Ernie,

 

Wow - this thread seems to be a hot one.

 

Please name the machine tool that you are using.

 

It might be insignifcant - but who knows.

 

Hang in there with this one - it will only build character.

 

Regards, Jack

[RandyN]

haha, Ernie you old trouble starter. While working at my previous employer, we had the "facet" argument many times. The facets were hard to remove on cosmetic show surfaces on the mold cavitys.

 

We used various software, Mastercam, Cim-Linc, Pro Manufacture, and tried adjusting surface tolorence, parameters in the softwares and machines, and I believe the biggest factor at the end of the day was the machine we were cutting it on. Filtering to arcs and the direction of cut went a long way though.

 

Next time I'm out in Calif. on vacation, I'll stop by and see how you are doing. Maybe you can make me an offer I can't refuse

[Robby GM]

Hi Tri-Tech 5-axis

When we finish large 3d surfces our finish cuts

are with a 30 mm ball end mill with .4 mm stepovers, yes you can see cutter lines in the surfaces but are too small to be a problem.

.001 mm's scollops on flat

.003 mm's scallops on 45

[Lucky]

There are many factors influencing the machined surface finish of a part. This thread has discussed many of them and my personal experience confirms about 95% of what has been previously stated. A technique that produces a good finish on one shape may not on another. Large curvature surfaces can be challenging.

 

Use tight tolerances for surface/solid model creation.

 

Use toolpaths that will permit arc fitting during filtering such as parallel with 0 or 90 degree cut direction and/or surface finish contour.

 

If you must use toolpaths such as flowline, constant scallop or parallel with cut directions other than 0 or 90 degrees - DO NOT FILTER. Filtering will lengthen the moves and worsen the problem. Use an absurdly tight toolpath tolerance and expect a big NC program. If your control cannot process the information fast enough new finish problems will result.

 

Many newer machines can automatically accel/decel based on a user specified contour tolerance. Complex surfaces with lots of fine detail and changes of cut direction benefit from a tight contour tolerance. Large curvature surfaces will be severely faceted; however, since the facets existing in the NC code due to the tolerances specified in Mastercam will reproduced exactly. Large curvature surfaces will look better if the contouring tolerance is larger. It has the effect of arc fitting or blending the straight line moves in the NC code. You may even get the best results by turning off the automatic accel/decel features of your control. With the tolerance loosened or off the blending effect will become more pronounced as you increase your feedrate. Every machine is different - you will need to experiment.

 

If your control supports NURBS input, a product such as Metacut Pro with a suitable post processor will allow full freedom in selecting a toolpath type without getting straight line movement in the NC code. I will be implementing this in the next few weeks.

 

I recently looked at a new Heidenhain control that permits the user to alter the dynamics of the machine's accel/decel based on prioritizing three factors: speed, accuracy and FINISH! The machine can alter the behavior of the servos on the fly to suit the curvature of the surface. The results are remarkable.

 

In summary, minimize faceting in your programs with tight tolerances, proper toolpath selection, and arc fitting. Reduce the effects of the remaining facets by reducing the accel/decel features of the machine control.

 

A long thread deserves a long post. Good luck.

 

[ 10-09-2002, 07:27 AM: Message edited by: Lucky ]

[P_Scott]

Tri-Tech,

 

There is one issue that no one has talked about and that is toolpath types. What version of Mcam are you using? V9 has a couple new toolpaths that may in fact help your search for the "cosmetic surface". If you are using older software, you might consider upgrading the software for improved control over the toolpath. It is an inexpensive way to improve the surface finish. If you do have V9, have you looked at the Surface-Finish-Project-Along 3D Blend toolpath yet? This combined with the tolerance and filter settings that others have mentioned may be exactly what you are looking for. Also adjust the Gap settings for a smooth transition of your stepovers. Instead of line moves, this alone could "clean up" the surface finish. With all the suggestions, download the file to the FTP and I'm sure there will be many hands working on the problem. Together we can find a solution. HTH

[Tri-Tech]

Wow, Thanks for all this infomation, keep it coming, You guys are great!

 

Randy, come on down. We need your expertise.

 

Back to the point.

I don't have a surface finish problem at this time, This is from past experience before V9, using all type of machines on all typs of work, doing many of the technics you guys refer too. And maybe V9 can cut it now. I will find out. I just don't see where I have control over how long the toolpath along cut line can be.

 

By the way, In the past when I tried Filtering with arcs. It did smooth out the along cuts but the across cuts would have digs (microscopic steps) that where also hard to polish out.

 

Does any one use controls that supports NURBS input, does it work? what is the advantage?

 

Best Regards,

Ernie

[Guest CNC Apps Guy 1]

Ernie,

 

I've used NURBS on a Fanuc 16iMA. It's main advantages are that it is a more precise method of defining the surface curve. Instead of having short line segments representing the curve, you have the entire curve being defined by Control Points, Vectors, and Knot Weights. Even Arc Fitting does not do as good a job of defining the curve. Granted, no software(as of yet) will take the actual NURBS data from the surface and translate that to code, it should not be too far off.

 

Currently you'll need to create an insanely tight tolerance/point dense NC file, then run it through NWD Filter to get the NURBS output. Yes it is a two step process but it is quite worth the effort and processing time. You have faster block processing time (1ms last time I checked) with NURBS and longer look ahead.

 

HTH

[Greg Williams]

James,

 

Where can I find this NWD filter that you speak of?

[kwolf]

You can find it at www.metacut.com

[James Barnes]

Ernie,

one very common technique for reducing facets and achieving class A surf finishes is to

machine in two directions.The second being perpendicular to the first.Most people say that will double my machine ! try telling that to Ford.

[Guest CNC Apps Guy 1]

Ernie,

 

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

 

JM2C