Lying about bit size to affect part size

[sbd1]

I may be totally off the mark here, so I'd like to hear how experienced users do this.

If I have parts being cut that need to be accurately sized, but are slightly off, I have been editing the bit diameter in my tool database & then recalculating the toolpath & then re-creating my part file.

Then I saw 'Proportions' in the FP fill-in sheet when loading a file & wondered if that could also work. Can I also adjust that to accurately make very small adjustments (ie: .01") to my toolpaths?

[steve_g]

Daren:

Use the offset tool... it accepts positive or negative numbers.

SG

[sbd1]

I assume that setting is in Partworks Steve? I use other software & I don't think I have that setting, but I do have an 'Allowance' tolerance setting that I believe does the same thing. And unless I'm mistaken, changing that would mean that I would still have to re-calculate the toolpath & then re-create my part file. I thought there might be a simpler way.

[steve_g]

yes that would require a recalculation of toolpaths.

The proportions fill is in percentage. When I tried it I had a hard time predicting where the part would be located on the bed...

SG

[sbd1]

When I tried it I had a hard time predicting where the part would be located on the bed...

Good point Steve. Looking forward to hear if there are any other options.

[knight_toolworks]

the best way if the drawing is accurate and you are doing a profile cut is to do the climb cut and a cleanup pass in the regular direction. If it is a pocket that is a bit tight and it is something you will be cutting over and over I would use the offset tool to adjust it.

[steve_g]

Daren
One more possibility... bits are sometimes not the size they say, especially if they have been sharpened! Put a mic on a few and see what you have.

SG

[garyc]

Daren...
If your parts are not cutting the proper size you have an error somewhere in your design/cut/motion system. Even tho you may be able to use cutter diameter as compensation, it would be better to find the root cause of the innaccuracy.

Tool diameter, cut parameters (feed rate, stepdown, bit type, cut direction), RPM, hold down, pinion gears and grub screws, machine adjustments, condition of the mechanical motion components, unit values and even ramp settings can affect part size.

If you check and verify each of the above to be accurate, or within specs, you should find the cause.

[MogulTx]

I would heed Gary's advice, but I also echo what Steve said: check the bit diameter. I have had a few that were off enough that I noticed a difference in material cut sizes. I use a big (40") caliper to check medium sized parts and a small caliper to check bit sizes if I am doing something of critical dimensions.

MGM

[sbd1]

I can now see this is opening a bigger can of worms than I originally thought.

I understand & agree with what you've said Gary. I've just finished weeks of reassembling, checking & adjusting the entire machine along with building a completely new table. I've done my very best to be accurate, but given that I only have a simple set of calipers & a dial gauge, I don't think I'm able to squeeze much more accuracy of it. And as Steve said, I see that my new 1/4" upcut 2-flute spiral bit isn't exactly 1/4" after all (although it's a little tough to measure).

Here's the results from a simple test cut today (see pic).
Actual bit dia: .246
Bit dia toolpathed: .24 (I changed it last week to .24 after .25 resulted in ~.01 oversized parts & I didn't know about proportioning. I should probably set it to the actual bit size & run these tests again)
Stepdown: .4
Tabs
Climb cut
.75 MDF

Test Cut 1
Part undersized by:
X .006
Y .01

Test Cut 2
Same toolpath but changed proportions on fill-in sheet when loading the part file
X proportion: 1.005% (2/1.99)
Y proportion: 1.003% (2/1.994)
Part accurate size

So I now see that I can get the results I want by running a test piece & changing the proportions, but is that how I SHOULD be doing it? If so, do I have to run a test cut every time I change bits?

[John David]

You should set the bit to the actual size and re run the test. It looks to me like you will be with in machine tolerance.
JD

[daski]

There are many things that will affect the final size of a part, even the sharpness of the bit will have an effect, new bit cuts, dull bits poiund. We found that we would do an accurate drawing, then do a test part using two pass system, first being almost all the way through, the second cutting the oinioskin. The 1/4" bit will deflect when cutting, plus the slop in the gantry, z axis, bearings in the router, resistance from the panel density, they all add up to a number that will remain fairly constant given the same situation in the future. We found that a 1/4" bit needed to be enetered as .243, climb the conventional cutting.

You are better figuring out what the cumulative number is and allow for it in the bit as opposed to a percentage,

[bobmoore]

You havn't said what material you are cutting or whose bit you are running. O flute bits should not be miced. You are much better off to lower them into the material you are running, raise it up and mic the hole diameter. Some plastics can compress when being run and then relax after the bit passes. There are reasons for tolerances in manufacturing and sometimes the customer needs to be reminded of them. Maybe have a company with a big gun CNC run some samples for you and see what there quality level is with the same material, no sanding, ect.
Bob

[sbd1]

Bob: I like your idea of drilling a hole with the bit & then measuring that, rather than trying to measure the bit. I did mention I am using a 2-flute bit in 3/4" MDF. Interesting info about plastics, but I'm not there yet. The drill hole size measured .247.

John: I reset the bit size to .247 & recalculated the toolpath & then recut the test block (see image of 2" test square). X is out by only .001 and Y is out by .008, which probably tells me that I need to address some play in my Y travel/hold system, but at this point in time I'm pretty happy with these.

Dave: I'm using a new 1/4" upcut spiral bit with two-climb cut passes. The results seem acceptable to me, but once I get more comfortable with everything I'll give the opposite direction cuts that you mentioned a try.

Thanks everyone for your advice & information. From this I've learned that I need to be more accurate with my bit size & that I can make changes to a parts' final size in 3 different ways:
1) By changing the proportions of the part file in the fill-in sheet.
2) By recalculating the toolpath with an offset or allowance.
3) Changing my bit size & recalculating the toolpath.