Class "A" Surface Machining

[Verisurf - Ernie Husted]

Does anyone know the best way to achieve a Class "A" surface finish?

 

We have a company requiring us to cut large car body tooling with Class "A" finishes. No benching allowed only a machined finish. Ready for polishing.

 

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.

 

Any tips would be appreciated.

 

Ernie

[Trevor Bailey]

the first thing i jwould look at when it comes to your finish, is the model you are working with. if you are getting facets, have your designer tighten uup the tolerance in his software before you get the file. this will greatly reduce the facets.

 

the number 2 & 3 & 4 thing is obviously high RPM, tooling, & feedrates. really tighten all filters in MC also. try to use a toolpath that will not cause the machine to "jerk" in transition moves.

[Guest CNC Apps Guy 1]

Well Ernie,

 

Facets can be caused by a number of factors not even related to Mastercam. "Class A Finish", this is totally non-descriptive. To me, surface finish HAS to be caled out as Ra, etc... Back to the point. Surface finish is often at the mercy of Ball Screw pitch which is almost NEVER even considered. This is usually seen with large radiuses. I've made a mold or two on a Mori Seiki SV-500 w/ Data Server running in HPCC mode that was down in what is usually considered grinding surface finishes. What contributed to the success of this project was

[*]Tight tolerance on Surface Creation (.00001)

[*]Tight Tolerance on surface toolpaths (.00005)

[*]Tight Tolerance on Filter using NWD Metacut Pro (.0001 if memory serves me correctly)

[*]Fanuc Dataserver (so I did not have to worry about servo lag and/or Data Starvation

[*]HPCC (Fanuc High Precision Contour Control that controls acceleration/deceleration to maintain contour precision)

[*]Good rigid balanced tool holders (Tecnara)

[*]20,000 RPM Spindle

[*]Robb Jack, OSG, and Sumitomo Carbide, Cutting tools

[*]High Speed Machining principles

[*]Mori Seiki's outstanding Machine Quality

[*]and Mastercam

These variables combined to put 2 mold polishers into aonther facet of Moldmaking of face being layed off.

If you want more specifics, post here and we'll continue dialog.

 

JM2C

[Tri-Tech]

I understand that tight tolerances and tight machines help out alot.

 

Without changing tolerances or machines, what I see is, some surfaces have a smooth finish and some have facets or line patterns.

 

What I am looking for is, why it is that some sufaces cut smooth and some do not?

 

I once had a model of multiple surface patches, after machining it, some of the patches where smooth and some where not.

 

I do not use filters.

 

Ernie

[Trevor Bailey]

it is the way the model is created that is giving you the trouble and facets. it all comes down to how the model was created and how tight of tolerances were used in creating that particular surface. not all surfaces are created using the same methods. there are many different techniques(sp).

 

i will say it again, tell the guy/gal you originally got the file from to send it to you agian with tighter tolerances set. i am positive that you will see a difference.

[Trevor Bailey]

it is the way the model is created that is giving you the trouble and facets. it all comes down to how the model was created and how tight of tolerances were used in creating that particular surface. not all surfaces are created using the same methods. there are many different techniques(sp).

 

i will say it again, tell the guy/gal you originally got the file from to send it to you agian with tighter tolerances set. i am positive that you will see a difference.

[Guest CNC Apps Guy 1]

quote:

---

I do not use filters.

---

Any particular reason?

 

Did you Analyze the surface and did it check out OK? Is there any way to re-model the surface somehow JIC it was corrupted during the transfer?

[Guest CNC Apps Guy 1]

One more thing, you can and will get different toolpaths from different surface types. I'm sure you're aware of this though, right?

[Greg Williams]

Hi,

 

I have found that almost all surface faceting issues are related to the model and the tolerance (or lack of it) that it was created under. The use of filters can help the problem by smoothing some of the high points but As the saying goes Crap In equals Crap out.

 

Firstly have the designer check his/her surface tolerance, then look into the more expensive variables such as machines etc.

 

PS What is a class "A" Surface finish?

[Tri-Tech]

I refer to a class "A" surface as one that is optically smooth. You have to use the light rays to see the diamond patten I'm referring to. it's most noticeable on some large curvature surfaces but not on all.

 

I'm sure it is a math thing. I tried all the different filters with no success. Filters remove points I need it to add points to the program. The problem is before the filter, I can backplot and save the lines. Then do Screen Endpoints and I could see the same patten as I do with the light reflection test of the cut surface.

 

This is for advanced users only, please.

 

Does anybody cut car body tooling that require class "A" surface finishes?

 

I need a toolpath with a uniform cut patten.

Is this a Mastercam problem or do all CAM systems have this problem?

 

Ernie

 

[ 10-07-2002, 09:55 PM: Message edited by: Tri-Tech ]

[Michael Reynolds]

Hey now, James was only trying to help!!!!!!

 

BTW James, nice beeneeeee.........!!!!

 

Respectfully,

 

Mike R.

[Tri-Tech]

Sorry, James

[Jack Mitchell]

Ernie,

 

I once quoted a job for a defense contracter.

This entailed me producing a workpiece that did not contain a finish tolerance on the part itself.

The tolerance was the relection from the finish - or there abouts.

The part was a radar reflector for some kind of weapon (We had to have an armed guard accompany us in order to view the prototype).

 

The finish you require could perhaps be obtained through polishing as opposed to trying to machine an improbable situation.

 

Yes, we do have the mathematical and mechanical technology to solve many tasks, I don't believe what you are after to be a realistic expectation.

 

Please do not take offense - perhaps I and the others misunderstand what it is you are looking for.

 

Regards, Jack

[Michael Reynolds]

I humbley agree, Jack. I don't think an optical surface is possible to machine using a ball end mill (without having a step over distance of about .000000000001) (just a guess)..

 

Mike R.

[Tri-Tech]

Thanks, Jack

 

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.

 

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.

 

The reason we still have contol over the across distance is because you can clearly see that the curvature tolerance doesn't work good on some surfaces, that's the same problem I see for the along distance. I think we need an option for maximum stepover for the along distance.

 

What do you think?

 

Ernie

 

[ 10-07-2002, 11:28 PM: Message edited by: Tri-Tech ]

[Craig Madsen from CM3D]

Hi, Ernie.

 

I believe that in the area where you select the chordal deviation in Mastercam you can also elect to use a 'along' distance. You could enter your .02" here.

 

Craig Madsen

[Tri-Tech]

Hi Craig,

 

I wish!

Where can I find that setting?

 

Are you having flash backs too?

 

Ernie

 

[ 10-08-2002, 01:17 AM: Message edited by: Tri-Tech ]

[Tri-Tech]

Old School Settings

 

New School Settings

[Greg Williams]

Ernie,

 

Are after a smooth uniform part with no visible deformititys such as facets or wave forms?

If so you need to look very hard at how the original model was created, In what system?, using what formula? and most importantly to what tolerance. Also how is the part translated into Mastercam, If you have used IGES, This may be your problem. To machine parts to a very high surface finish all of these aspects need very close examination.

[Roger Peterson]

When machining a part designed in a cad package that also had some "professional manufacturing" capabilities I could not come up with a satisfactory finish with my .016" ball endmill. When machined with the "professional manufacturing" software the finish was still horrible, after some remodeling at tighter tollerances the finish was spectacular. In Mastercam it was much better but still not good. I am going somewhere with this. This brought up a lot of questions. Basically it came down to modeling tollerances and file translation. This was in V8 and the IGES file was now the problem. I tried several other methods and results ranged from the better to spectacular. STEP files are a great universal alternative to "IGUESS" files. This was not on an expensive machine with only a 10,000 rpm spindle. I don't want to kick a dead horse and I don't know if the sf your looking for is attainable but good luck.

[Guest CNC Apps Guy 1]

True, the Model should be the first source to look for trouble, first because it is the least expensive to deal with if there is a problem, but you shouldn't rule anything out. I mean if you're trying to hold microns on a Fadal or Haas, sorry to tell you but you're exceeding the capabilities of the machine by about 10x.

 

What system was the model designed in? I've had some problems with faceting on EXP files from CATIA, but have not had any faceting problems with MODEL files.

 

JM2C

[cadcam]

Have you tried setting the tolerance setting to 1:1 ratio and useing the cut tolerance from .001 down to say .0001 or more?

 

JM2C

 

[ 10-08-2002, 12:43 PM: Message edited by: cadcam ]

[Robby GM]

In auto die work there are 2 types

of sheet metal parts.

Black metal = parts not seen by the eye

( supports, inner hoods etc )

Class A surface = are parts you see

outer hood, outer door etc

 

Class A surface refer's tpo sheet metal part

not surface finish of die it self

 

Robby GM

Metal Fab ,GM

 

[ 10-08-2002, 01:38 PM: Message edited by: Robby GM ]

[Tri-Tech]

I'm sure its not a machine or model problem.

 

What happends to toolpaths of some large curvature surfaces, even when the cut tolerance settings are set down to .0000001" is that the along cut points are still separated by more then 1/8". That is a straight line. Those straight lines show up on the polished part.

 

Filters remove points making the lines even longer.

 

I'm I getting the point across?

 

Ernie

[cadcam]

quote:

---

I'm I getting the point across?

---

I get your DAM Point. I like every one else is trying to help.

I guess your are getting frustrated with this.

This does not help when you get this way with us that want to help, Why not call the main office and ask support if there is something else you can do.

 

[ 10-08-2002, 02:11 PM: Message edited by: cadcam ]