Thin wall help

[romer]

I have a job that requires a number of finished thin wall contours between .020 and .040 thick. I have been playing with the finish settings and using the spring feature and wear compensation.

 

When I cut test parts, I'm getting inconsistent wall thickness and am having trouble holding tolerance. I keep cranking in more and more cutter comp but I'm afraid the cutter will all of a sudden "bite" and scrap the part.

 

The walls are between .250 and .500 deep in

6061-T6, and none are closer than .375 so I dont think cutter rigidty is a factor. I have some low temp solder coming tomorrow but have never used it.

 

Any suggestions on feeds, speeds, cutters, techniques, use of solder, magic chants, etc. would be appreciated.

 

Thanks,

Romer

[Fig sign]

In general ,it dependes how really nonrigid walls you have .

What would I do if I have a high thin nonrigid walls ?

I will devide advices on two parts technology and programming .

1. technology - use the smallest available rigid mill.

The smaller the mill the smaller bending momentum.

Use CONVENTIONAL MILLING ,not climbing.

Climbing pulls a part under mill,conventional push it on the opposite direction !

Maximum you `ll need to take 2-3 finish passes more in case of conv.,in climbimg you are risking to broke tool or part or at least to mill more

metal that you need !

When you use long mills look on the proportion lengt/diameter - 10 or more is a long(nonrigid) tool .

In such a case don`t be afraid to low down RPM and feed ,especially if you mill corners.

Try 50 -40 % rpm and feed 50 % as a start values .

When you hear shrieks of a mill go down with rpm!

The feed you can down less , in lower rpm it is ok.

And always leave "meat' for a mill ,don`t leave 0.01 mm for finish !

So in technology I will advice conventional milling , small tool and lower rpm and feed.

2.programming

a.You can mill your walls with a little takeover and many passes.

b.

You can mill a pyramide .

you mill only a little height of a wall finish.

Let us say that the wall thickness is 0.5 mm and heigh 15 mm

in rough condition it`s thickness 1.5 mm - Rather thick wall.

You miil half finish and finish first 5 milimeters, then the next .then the last like a ladder !

If you have very thin wall like height 15 mm ,sizes X50 and y 0.5 ,never mill the thickness x50 when y0.5.mill it before when yis 3-4 mm .

In other words ,sometimes is good to differ milling of sides and not to mill all sides like 1 contour.

 

IHTH

 

Iskander teh long mills thin walls miller

[TheePres]

Only 1 thing to add to Plastav's comments:

Use 30 or 45 degree helix cutters.

[CAM-mando]

If using carbide, I agree with the hi helix. HSS, the Internationsl minicuts or similar tools are good for pocketing.

 

Consider Roughing and finishing at each Z level before proceding to the next Z level. Cutting in this manner the free height of the wall will only be the roughing depth of cut amount since the wall is suported by the material below it. For deep pockets or walls consider relieved (necked) end mills that have clearance ground on the diameter just beyond the depth of cut. For multi pass depths rubbing will be eliminated. Lastly, in some applications I have had better luck taking a heavier radial depth of cut on the last pass. Essentialy no real finish cut. Again the wall is supported in front of the cut. Sometimes combining this with the rough / finish at each Z approach can yield decent results.

[Fig sign]

quote:

---

For deep pockets or walls consider relieved (necked) end mills that have clearance ground on the diameter just beyond the depth of cut.

---

There exists one nice trick for roughing deep pockets or inner contours:

in pocket->depth cut -> tapered wall you can put tapered angle and you will do tapered wall !

No need to relieved tool !

But this method will not work in outer contours :

the taper will be in other direction and you `ll

undercut your part.

 

And one more thing related to my former article :

Try to use long mills with a short flute rather then with a long one - more rigid !

[titleist]

use a high helix end mill and leave .002 for finish pass

[Jimmy Wakeford from Barefoot CNC]

What size cutter are you using, depth of cut for main pocket, depth for thin wall option?

 

Jimmy

[Fig sign]

In trick that I mentioned the pocket must be without islands .

Anyway it is very easy to build drafted surfaces and use surface->rough pocket job without relieving a tool .

[CAM-mando]

plastav,

 

you are correct in your statement that tapered wall (or simply programing individual contours with increasing stock to leave) will allow positive clearance above the depth of cut, but the minimal effort required to relieave an end mill is a simple toolroom task that pays big dividends in certain applications. I use it in penciling deep vertical walls and in the application described when I dont want to take a true "finish pass" that would be required to remove the taper cuts or steps.

 

I agree on the short flute length, Robb Jack has the "Tuffy" mills and others offer neck relieved short flute endmills for this purpose. They work quite well in this application.

[Fig sign]

I don`t deny releaving.

I do it myself when I must (I can grind a reliave if I need).

I simply try to minimise it`s use :

reliaving does the tool more rigid!

When you have tool diameter 1mm and lenght 10 proportion is 10 the tool relieved to 0.9 proportion is 11.1 !

And because I am in molds production most of my parts are single ones I use tools in many parts and relieved tool you can not put in the toolholder with a short lookout !

 

The deep miling and drilling also is an interesting thing to do especially when you are new to it and not so scaring as it might look at first !

 

 

iskander teh crazy man for crazy parts !

[CAM-mando]

quote:

---

nder teh crazy man for crazy parts

---

[Guest CNC Apps Guy 1]

quote:

---

Consider Roughing and finishing at each Z level before proceding to the next Z level.

---

+1000

[Müřlıń®]

romer...

quote:

---

I have been playing with the finish settings and using the spring feature and wear compensation

---

Is this feature with Ver 9.1 on the thin wall function?

 

Havent found any of those fileds on any menues on Ver 9.0.

 

 

Murlin

[romer]

Thanks for all the helpful replies guys.

 

Experimenting with various suggestions finally did the trick. Conventional instead of climb cutting was the biggest improvement.

 

Murlin,

 

The spring and wear comp setting are on the roughing/finishing tab of the pocketing function.

 

We went from 8.1 directly to 9.1 so I don't know if it is in 9.0.

 

Thanks again,

 

Romer

 

[ 07-23-2003, 06:37 AM: Message edited by: romer ]

[Ken Erman from CNC Software Inc.]

Thinwall settings, including spring passes is a 9.1 feature. Is the thinwall option usefull for your part?

 

An iquiring PM wants to know...

 

Thanks,

 

Ken

[Müřlıń®]

PMguy.....if the Spring function were to be added to Surface Finish Contour, woah.... that would be awesum....

 

Sometimes, you know that your tool is going to deflect a certain amount.

 

I end up lying about my cutter size when I use Leftover after a Finish Contour that is deflecting alot in order to get the two cutterpaths to have a nice transition.

 

I try to machine with the "least" amount of toolpaths possible in Operations.

 

 

 

Also, Surface Finish Shallow needs a "bottom" tool wear function for machining Shallows with the same tool that you just used for Contours.

 

I want to be able to control my tool deflection and wear on all algorythms.

 

I might have to add this to the wish list for Ver 10

 

 

Murlin

 

[ 07-23-2003, 09:10 AM: Message edited by: Murlin ]

[Ken Erman from CNC Software Inc.]

Murlin,

 

It was hoped to get it in the 9 series, but other obstacles intervened. I still have it on my list for X.

 

PMGuy

[Müřlıń®]

 

More reasons to upgrade to X......

 

 

Murlin

[P_Scott]

romer,

 

To go along with what Plastav and others have said, there is a function in the Depth Cuts button of a 2D contour or Pocket operation. It is called "Depth cut order" and has been around since V8. By selecting the "by contour/pocket" radio button in this box instead of the "by depth", you are essentially doing all the roughing and finishing at the same depth for all contours/pockets chained for this operation. Doing exactly as CAMando suggested here:

quote:

---

Consider Roughing and finishing at each Z level before proceding to the next Z level.

---

It may also help to rearrange the chains so that contours/pockets aren't right next to each other. You can accomplish this by left-click/dragging the chains in the Chain manager of the operation. HTH

[Fig sign]

+1 for Peter !

I use it sometimes .

But I go further , I do rough tool & finish tool 1 step , then rough tool & finish tool next step and so on .

Like a ladder .

 

There are endless tricks that can be implemented like fails walls and so on.

 

Every part has it`s one gimmick .

 

[ 07-24-2003, 01:18 PM: Message edited by: plasttav ]