Machining precision parts involving replaced tools and the need to modify CAM?

Hi Im a noob machinist doing it for hobby. I got two questions.

I'm wondering, what is the proper way of ensuring a single machined part is manufactured to precision the first time around based on offloading it all to automation? (say fairly low tolerance of 0.005mm). I mean, is it the 'customary' way to measure the actual diameter of the cutting tool first before programming the G-code to machine the part? So if you have a fancy laser gauge you can measure the tool diameter (you have to measure at the cutting RPM too right?) or for hobby/lower budget people without those renishaw laser gauges, do you just plunge mill a hole into the intended material then precision measure that hole?

I mean to ask, is it the only proper way to do precision stuff is to first measure actual tool diameter (laser gauge or mill then measure hole), before going to the CAM side to program the G-code by inputting the actual measured tool diameter?

My second question is along the same lines. If you are in a mass production environment, and one that ultimately involves tool replacement due to broken bits, how do you ensure your G-code is usable for this new tool since there may be some tolerance in the tool itself from the manufacturer. In other words, the G-code program you spent a lot of time on for one particular tool, may not be a great fit for the replacement tool which may have a different cutting diamater. In other words, for mass production relying on automation, do you need to re-program the part every time a tool change is done, in order to maintain low tolerance manufacturing?

Actually it's fairly simple...

...You write your program to zero offset and G41,G42, G40 as necessary. In the machines you use the tool diameter (or radius) and height screens to describe your tools and adjust as needed for size and cutter wear.

If these "G" codes are not familiar to you , you'll need to study and learn them, and your machine's ability to use them.

Steve

And yes, the best way is to precision measure a sample part, as the actual cutting conditions represent the sum total of all errors and what you measure is what you get.

The feedrate used to interpolate a hole will affect the measured diameter. That is one example where measuring the tool does not really tell you what the result will be with a given toolpath.

And for lathe turned parts, the only way to really verify the final tool position is to measure what diameter it cut and compare it to what was commanded, and then adjust.

For one-off parts, you can choose to deliberately post the sample program with generous finish amounts left. You would in this instance, like to leave a decent amount for a final run through with the tool offsets adjusted. In effect, duplicate the finish cut amounts so you get the same tool deflection on the final finish cut.

noobimachinist said:

(say fairly low tolerance of 0.005mm).?

Click to expand...

Do you consider that a low tolerance?

Thanks for responses.

Does tool compensation always work for all even complex geometries? And does it involve manual modifications sometimes? Say you are creating a part involving running the endmill along a straight line and then back to create two 'cliff-edges'. Does tool compensation know to shoot to the left on the forward pass and then shoot to the right on the backward pass to compensate?

Do you mean interpolate a hole bigger than the known tool diameter to measure dynamic cutting performance with larger radial forces on the tool by moving the cut, or simply plunge the end mill into a material to get the idea of cutting diameter?

behindpropellers said:

Do you consider that a low tolerance?

Click to expand...

I guess for hobby stuff I dont think i can even get that. My gauges dont even measure to that level.

What should be a low tolerance figure?

I do!!

+-.000197 is pretty low tolerances for lathe and mill

re: general "high tolerance" has come to mean "close and difficult" and "low tolerance" always sounds vague to me, but apparently means "easy". So I talk about tight or close rather than "high" and loose or easy rather than "low".

re: noobimachinst - tool comp does nothing more than offset the positioning of the tool by the size declared for it in the tool table, said size most likely measured with a tool setter on the machine or by a human using a tool setting station of some kind. the comps have to be told whether to offset left or right. you might take test cuts and then measure the result, and change the offsets to reflect that. some controllers will allow you to condition the offsets for wear and age. but it's just table of nubmers for the tools, said numbers being used to offset left or right.

it doesn't make sense for all geometry - some kinds of 5 axis work for example.

so one practice is to measure tools carefully, and then extract those sizes and feed them into a cam system. if you are going to adjust for actual cutting behavoir, do that before loading the offsets into the cam program.

or, generate (via cam or hand) code that uses offsets - then changing the offsets in the tool table will automatically correct the program.

I hear that term too, i.e. 'close tolerance'. But I duno if low tolerance is necessarily used incorrectly though. Tolerance in laymen terms in life is kind of 'how much shyt you are willing to take'. So when someone says they have low tolerance for crime, it means they dont take BS lightly.

So low tolerance in machining sounds to me, you don't easily accept things that are off. Which translates to a lower 'number' for the tolerance which works out. So +/-1mm is high tolerance because you accept 1mm deviation from design. But +/-0.005mm tolerance is low tolerance because you reject the part even if it is just 0.006mm off the design?

But I understand the wording can get confusing too. It almost sounds like 'low tolerance' is 'low standard'. I guess it is describing the quality of a negative. We tend to associate or are used to the quality of a positive. Such as 'good quality' instead of 'low shyttiness'.

Yeah it makes me wonder about the multiaxis stuff for tool compensation. Say you are milling a circle pocket. There are two arcs. If your tool is larger than desired, you can specify manually in the CNC control software the left arc compensate to the right and the right arc compensate to the left. Is this prepared CAM side to know this? What if they do a stupid thing where they compensate both to the right or left?

I guess for simple geometries or 2.5D stuff it might be easier to ensure tool compensation always works, but for complex stuff or multiaxis, is this always the most fool proof method, or is the most precise method to re-CAM the part after accuracy measuring tool diameter?

Semantics

The manufacturing industry has it's own definition of" high tolerance" ( tighter tolerance... i.e. .005m... harder to achieve more costly) and "low tolerance" (wider more open tolerance... .145mm...easy to achieve and a lot cheaper).

It's technical semantics, you'll have to get use to it.

" Say you are milling a circle pocket. There are two arcs. If your tool is larger than desired, you can specify manually in the CNC control software the left arc compensate to the right and the right arc compensate to the left. Is this prepared CAM side to know this? What if they do a stupid thing where they compensate both to the right or left?"

Not enough path detail to answer. But, with the information you gave I would guess two possibilities:

The machine "will look ahead" and give you an error message... the pocket to cut, is smaller than the cutter.. (better the machine control the better it is at this detection, but most newer will let you know you told it to do something it cannot do).

The other example is that it will only cut in until it intersects the arc on the other side leaving you still with material to be removed.

In rare cases, some features may need to be reCAM'd. But in most cases this is a matter of over-engineering.

Remember... that not only is Form, Fit, and Function the rule...cost is a reality... and it is the king over all else.

Steve

Use the terms tight/loose instead of high/low when it comes to tolerances. Less likely to cause confusion.

Your CAM software should output the correct cutter comp / wear comp g-codes, G41 for left and G42 for right.

You set your tool wear compensation, just a few thousandths or ten thousandths of an inch, and the G41/42 will offset your toolpath.

Laser tool measuring gages are for process reliability - detecting broken or worn tools, not for accuracy. There is no way around measuring an actual part.

Tools inevitably wear out, but you can slow down the process by using dedicated finishing tools, dedicated finishing tools for specific features, and tools that are designed to last longer, e.g. PCD inserts for cutting aluminum.

There are also in-process gaging solutions available, such as Marposs gages for cylindrical grinding and air gages for Sunnen hones. The machine keeps cutting until you hit tolerance.

When I saw this earlier today, "low tolerance of .005mm" on a mill. I was thinking the worst.

Tight/Loose that's the way to do it. You pay more for something that is tight than you do for something that is loose... Make your
own analogies.

As for worrying about exactly what diameter your cutter is running while sitting there and spinning in free air.... That means roughly
approximately shit.

We have this huge problem... We are working with metal, seems like good stuff, rigid, doesn't move. That's wrong, metal is really
just like Jello. A bit stiffer than jello, but still jello. Not just the part we are cutting, but the machine we are cutting the "metal jello"
on. Also the tool holder, the actual cutting tool (carbide does bend, not a lot but it does).

So, your cutting tool is bending, your part is bending, your spindle is bending, your entire machine is bending.

Just got to play with it, every tool, material, machine and cutting parameter combination has its sweet spot.

As for programming... already been said, "compensation". How do you get it nuts on your first shot, test cut if you aren't
familiar with the parameters(machine,material, tooling) you are working with. So you want to take a .010 finish cut, rough within .020, take a .010
finish cut. Its .0005 under, move that finish tool over .0105, comp the rough tool .0105 and just run your finish cut, then run out the rest of your parts.
Keeping an eye on them of course.

Just to add......
When dealing with +/- 0.005 mm tolerances, add the following variables to those noted by everyone else:
Coolant temperature
Machine temperature
Part temperature
Tool temperature
Residual stresses in the material
Induced stresses in the material
Cutting tool edge condition and degradation over time and the effect on stresses in both the machine and material
Cutting tool geometry
Nano level shear zone physics of the material to be cut
Harmonics and vibration
Just to name a few.......

Exactly, one would have to have a machine with less than a hundredth millimeter play in the first place. When my boss stressed the fact that a customer demands ± 0,02 mm true running with parts I tried to explain that we have ± 0,01 already within the apparel. Boss also had me make mandrels by hand because he didn’t want to buy any.

Milling to ± 0,005 mm is possible but stupid. If I have grooves tolerated like this I rough them out and then go grinding or lapping. CNC will never replace the machinist’s deliberation who needs sound knowledge of all procedures. It’s good to master G-code programming and everything but as a mechanic, hobby-wise as well, it is you who decides how to achieve something.

You can produce perfect flats with three pieces and a scraper (and lacquer).

Avsfan135 said:

I do!!

+-.000197 is pretty low tolerances for lathe and mill

Click to expand...

You do realize that he was talking about mm and not inches?
If yes and the tolerance you've given is in mm then what industry are you working for?

zero_divide said:

You do realize that he was talking about mm and not inches?
If yes and the tolerance you've given is in mm then what industry are you working for?

Click to expand...

You do realize that .000197 is the inch equivalant to .005mm

We machine to +/- 0.005 mm on roughly 60,000 parts every day. +/- 0.001 mm on bores. Process stability is king at these tolerances.

Mechanola said:

You can produce perfect flats with three pieces and a scraper (and lacquer).

Click to expand...

What is this method called (So I can search for books/references to learn more about it). I'm sure the method you're talking about requires a lot of labor, but I'd still like to learn about it.

MargoTool said:

You do realize that .000197 is the inch equivalant to .005mm

Click to expand...

Ooops sorry, my bad. i saw a 5 in there in in my mind expected it to be 5 hundredths.
Just because he said he was working in a garage.

I gather on a good machine its quite easy to get it, but quite hard to keep it.
Spindle and ballscrews grow, coolant warms up, moon changes its position in the sky.

I remember our lathe guys kept Lathe spindles running dummy programs just to keep tolerance.

Sometimes lapping surfaces dont produce flat surfaces, but often there can be 'bowing' if mating pieces are lapped in place.