1st use questions about settings and outputs - XL timing pulley

[Matt P]

Hi All,

I'm just starting with the software. Looks quite impressive.
My first attempt with the software will be to make some XL timing pulleys.
I have tried to do some searching on the forum but haven't really found what
I'm looking for - which probably says more about my search skills/keywords than
the info on the forum. Anyway...

I have made and output a 72 tooth XL gear (wheel). It has stated that the Max mill dia is 0.0508
I have found and reduced the gear point distance setting to 0.0001. This makes the image look smooth.
But when I export and import to solid works all the curves are approximated by 0.001" lines.
Also putting in a curve that approximated the lines, the 0.0508 tool is too large to get into the bottom
of the filets that make the bottom section of the pulley.
Also, if I fix the flat sections of the pulley, putting in a tangent curve does not give the same diameter
of the piecewise linear approximation -< tangent =&nbsp; 0.0207 vs curve fit = 0.024
Also, Gearotic says the gear dia is 4.5637. If I put that diameter of a circle into the part is come inside the
flats of what was imported from the dxf.

So, I'm wondering, what am I doing wrong here?&nbsp; I'm suspecting I've got some import issue in Solidworks.
Also, is it not possible to have the pulley output with curves, especially since Mach3 can support that?
Should the curves/filets not be tangent to the flats?

From a design standpoint, does it matter how deep the bottom of the inner diameter is?
Could this not be adjusted to allow for a larger diameter cutting tool?
From what I've seen, the belt doesn't seem to touch this.

Thanks - Matt

[ArtF]

Hi Matt:

&nbsp; &nbsp; &nbsp; &nbsp; Welcome to the group.

>> I have made and output a 72 tooth XL gear (wheel). It has stated that the Max mill dia is 0.0508

&nbsp; Im afraid when it comes to the timing pulleys, the max mill diameter is a guess the program makes. This is because the timing pulleys are not a mathmatical formulaic curve, the curves in Timing pulleys are really a concatenation of curves specific to the specififcation of that pulley. XL's I think are about 5 curves tied together as I recall.

>>I have found and reduced the gear point distance setting to 0.0001. This makes the image look smooth.
But when I export and import to solid works all the curves are approxima ted by 0.001" lines.

&nbsp; Gear Point distance has a limiting factor. In the case of the gear your making it could very well be that internally GM is using .001 as its distance.
.001 on a timing pulley should be tight enough for any case where a pulley is made. ( Or so I figured when setting it up. ).&nbsp; If its not enough though,
I could make it tighter resolution, but I suspect its not required except for extremely small pulleys.

>>Also putting in a curve that approxima ted the lines, the 0.0508 tool is too large to get into the bottom
of the filets that make the bottom section of the pulley.

&nbsp; This can be quite common with timing teeeth that have acute angles at their root. If you use the smallest mill you can, its usually not an issue
&nbsp; as far as I know.

>>Also, if I fix the flat sections of the pulley, putting in a tangent curve does not give the same diameter
>> of the piecewise linear approxima tion -< tangent =&nbsp; 0.0207 vs curve fit = 0.024
>>Also, Gearotic says the gear dia is 4.5637. If I put that diameter of a circle into the part is come inside the
>>flats of what was imported from the dxf.

&nbsp; The diamter reading may be a bug, I will check that out. Timing pulleys have pitchlines that are larger than the outide diameter
&nbsp; of the pulley, so the statistics generator may be getting a bit confused. Im not sure what you mean by the first part on
&nbsp; fixing the flats or the tangent curve. It sounds liek your dealing with pretty small numbers.. see if you can drop me a
&nbsp; snapshot showing the issue. Im always willing to look at corrections, too many pulley specs are purposely obfuscated in the published specs.

>>So, I'm wondering, what am I doing wrong here?&nbsp; I'm suspectin g I've got some import issue in Solidwork s.
>>Also, is it not possible to have the pulley output with curves, especiall y since Mach3 can support that?

&nbsp; Sorry, but that isnt possible. While the Gcode could be arranged that way, all the data in GM globably is created as contours.

>>Should the curves/filets not be tangent to the flats?

&nbsp; No. All the various pulley specs specify radii and fillet centers sometimes by formula ( rarely) others be design to very unusual positions.
They do this so that as patents expire they can slightly change such things and create a new patent ( New and improved ). As a result, things
like the fillet centers and such are prescibed to a location as per the spec. and can easily be nontangent to any flats ( if flats exist ).
&nbsp;

>>>From a design standpoint, does it matter how deep the bottom of the inner diameter is?
Could this not be adjusted to allow for a larger diameter cutting tool?
From what I've seen, the belt doesn't seem to touch this.

&nbsp; Generally speaking, wide tolerance can be seen in practice with most gears or timing pulleys, but pulleys in particular. Most belts
&nbsp; do not touch the bottom of the roots, and as long as the tooth pitch is correct ( That IS important ) and the general form of the tooth
&nbsp; (width spacing ) is correct, then the actual fillets and roots tend to be pretty tolerant. This is why many find one type of belt runs fine
&nbsp; in another type of timing pulley. Not always, but often enough. :)
&nbsp;
So let me know if you find this confuses the issue, or if you want to drop a snapshot showing me any tangent issue. Ill list to
investigate the pulley diameter reading, its probably showing a spur of similar spec, the statistics generator does get fooled at
times, but the end tooth profile at the min point distance the program will accept is usually a toothform thats as accurate as one
should need. I can increase it if needs be though.

Thanks
Art
&nbsp;

[Matt P]

OK - still trying to wrap my head around all this - the way the teeth are formed, spacing, etc.
So, I figure the best way to learn is just to try cutting some.

Now I have other issues to work through. Namely the small diameter endmills.
Using GWizard to try to find some feeds / speeds, even just getting down to a 1/16" mill,
with full radial engagement, I either have problems with tool deflection or chip load or speed.

So, I'm hoping those that have gone before can impart some experiential wisdom on what has
worked for you.

Thanks - Matt

[ArtF]

Hi Matt:

&nbsp; Ill add my two cents worth.. :)

&nbsp; Cutting tight shapes has always been such a hassle. Making a gear too small will make it very hard to make. Obviously, an end mill must
be small enough to fit the tooth, though if its only slightly too large all that will happen is the trochoidal area will less defined, often not a serious issue with meshing. The true importance is that the tool doesnt cut off the other side of the tooth its cutting. Tool deflection, chip load and such is often dealt with
more with cut per pass, whith a small one you can up the speed of the tool ,even a small one to get the chip load you need. ( Going too slow is definitely
the norm for people having the most trouble. ). When I have to cut such gears, I use very small cut depth with a lot of passes. Its terrible how low
a depth you sometimes need to use, can take forever to cut one. ( By the way, on 4th axis work the tool can be somewhat larger than in 2d work as the
roots can still get cut by the edge of the tool's tip. ).

&nbsp; Getting the proper chip load in 2d work does require you to get at least close to the speed specified by the tool, and often the only way to
accomplish it is with very small cut depth increment. Over the years the most common error people hit is going too slow when the alternative seems to
be breaking the bit. Often tables , while great to show spec operation wont solve the issue, often times you simply need to cut some tests at various
speeds and depths to come up with what works for that particular material and bit.

(Sorry if this is too simplistic, you never know from what perspective someone is speaking. )

[Matt P]

Art,

Thanks for the insight - it is appreciated.
I'm new to all things machining - but learning.
So, all input is welcome.

I hope others will chime in with their experiences.

Thanks - Matt

[John T]

I work exclusively in wood and primarily baltic Britch plywood. My spindle is a Wolfgang Spindle belt driven with a 12 volt Axial motor. (About 50 watts)&nbsp; So i'm definitely on the on the "light weight" side of things.

When working with a 1/16" up cut router bit I work at 50 inches per minute, 0.070 inches per cut.
When working with a 1/32" up cut router bit I work at 30 inches per minute and 0.020 inches per cut.

Certainly no rule or anything but it works for me.

[Ken_Shea]

Matt,
Curious
What end mill size/type are you going to be using and what did GWizard suggest for&nbsp;
RPM
DOC
FEED
Chip Load

Thanks
Ken

[John T]

Hi Ken,
I can't be a lot of help here because I don't use the GWizard,
My spindle is fixed RPM&nbsp; and I've never used the other parameters - my variables are simply those available in Mach 3 motor tuning are the tool specifications in Gearotic and that's simply because that is what works for me - not very sophisticated i'm afraid..

[Ken_Shea]

Thanks John,
Was curious on how the calculations compared to different calculator.

"what works for me" is mostly what matters.

Ken

[Matt P]

I'm still working on this. Having some conversations with Bob over @ cnccookbook.
I'm planning on running tests on some 5052-H32 AL scrap that I have around.
But ultimately I'm planning on making these out of 6061-T6.

What GWizard is telling me -> see attached screenshot.

I'm hopeful these settings can work.
I'll post some more screenshots as I work things through both of the settings / cad / results.

Thanks for the help and encouragement - Matt

[ArtF]

Matt:

&nbsp; Calculated entries are a good place to start, but always consider them suggestions to start with.. Ive found over time that almost everyone
uses in the end "What works". Bobs suggestion to try scrap is a good one. Various bits vary widely in terms of recommended chip loads and
real life usage causes variation even higher. For example a set spindle spped changes htings quite a bit as the calcs are not necessarily linear
so experimenting is the best route..

Art

[Mooselake]

I work exclusively in wood and primarily baltic Britch plywood. My spindle is a Wolfgang Spindle belt driven with a 12 volt Axial motor. (About 50 watts)&nbsp; So i'm definitely on the on the "light weight" side of things.

When working with a 1/16" up cut router bit I work at 50 inches per minute, 0.070 inches per cut.
When working with a 1/32" up cut router bit I work at 30 inches per minute and 0.020 inches per cut.

Certainly no rule or anything but it works for me.

What kind of bits are you using, John?&nbsp; I was getting less than half those speeds cutting at a measured 15-20K rpm with a relatively comparable Paul Jones spindle, and using surplus PCB 2 flute endmills, mostly limited by cut quality in my cheap lauan plywood.

Kirk

[John T]

Hi Kirk,

I get most of my bits from
http://drillcity.stores.yahoo.net

The close up of these bits makes them look pretty aggressive but they produce a nice clean cut for me, in fact I can't see a surface difference between them and their end mills.&nbsp; I've used the fishtails but really don't have an opinion on them.&nbsp; A lot of the "demonstration" work i'm currently doing is in MDF which cuts like butter - very nice.&nbsp; When I switch to Baltic Birch I will have to modify some settings but not usually very much&nbsp; (its the glue in the plywood that causes the problem)&nbsp; If I'm carving hardwood with a nice close grain like maple then the normal settings usually work just fine.

I have used many re-sharpened bits and drills but I can notice a difference both in their ability to cut and their length of life.

[thinkntink]

One of the major problems with cutting wood (hard or soft) or wood products is that the density and cutting resistance from point to point is not homogeneous. To add insult to injury, these properties can change from day to day is response to humidity, temperature and the age of the material. This is one of the reasons that you will never see a comprehensive "Feeds and Speed" chart for cutting wood. We use G-Wizard almost every day when we are cutting metal and it is indispensable for a small shop. It is an amazing tool.

However, it's recommendations for cutting wood, especially with small tools, are at best, low balled approximations. For a given RPM, the feed rates are consistently low, often below the sweet-spot for cutter / material combination you are using. A more accurate, albeit empirical approach is to conduct a simple sweet-spot test to determine unequivocally that optimum combination of feed and speed. Go to:

&nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; &nbsp; http://www.precisebits.com/tutorials/ca ... speeds.htm

A pretty good rule of thumb for micro-tools (dia < 0.125", 3.18mm) is to:

• multiply the tool diameter by 0.04 (4% total chipload)
• multiply the product by the speed (RPM)
• if your diameter is in inches the result is the MINIMUM feedrate in Inches Per Minute
• do multi-pass cutting cutting 1 bit diameter deep per pass

Operating in the sweet spot will virtually eliminate breakage and can extend the life of the cutter up to 5X. As an example, we routinely cut Baltic birch plywood with 0.0280" cutter at 120 IPM @ 24 KRPM, at 0.056" deep per pass. Typical bit life is 7,000 to 10,000 inches.

All of this assumes that your system is in good shape and that:

• TIR[sub]max[/sub] < 0.001" measured 1.0" from the face of the collet
• Total backlash < 0.001"

Ron Reed

[BobL]

Ron;

Thanks for sharing, I agree on building your own toolbit feedrate tables to prolong life while trying to optimize that sweet zone area. In my case anyway, being a hobbyist, often no two cuts are identical nor do I use the same media consistently, so roughing it is often the way of life.&nbsp; I use this table to get in close proximity, then I use that albeit empirical approach with respect to the bit size and depth to look at the chips I generate in determining my optimum speed. On most media types I can cut on my table, being wood, plastic and soft metals, often I'll sit between the 25 to 60 inch/minute range statistically. Anyway a good rule of thumb to follow, fine powder, melting or blackening of the bit usually indicates your speed is too slow, warm even size chips is perfect, and broken bits usually means your going too fast. lol


Cheers
Bob
;)