Cutting marine ply gingerbread

[edp]

Have been asked to quote on a large run of 8" wide gingerbread fascia cut from 1/2" marine ply, Would really appreciate any suggestions as to type of bit and feed speeds - am looking for minimum sanding (read none)after cutting. I have had some problems in the past cutting this type of marine ply with tearout on the face veneer which takes forever to fill and sand. The minimum radius in the rather simple pattern is 1/4" so a 1/2" bit would be ideal for the cut. The top edge of the fascia is straght, the bottom 2 easy joined radii with a heartshaped pierced cutout on 8" centers 2" from the top edge. I have a PRT96 with a good vacuum hold down system so holding the sheets is not a problem. I have a feeling a ply boatbuilder would know about this sort of thing.

[davidallen]

I haven't tried marine ply but on other types, a downcut shear or spiral has given good results. I've tried a compression bit but unless you can cut the full width, you start with an upcut bit which tears the edge.

da

[srwtlc]

I've used an Onsrud 3/8" compression spiral with good results. The upcut portion is only 3/16" I believe, so you can easily keep the downcut flutes below the surface with a full depth cut. Feed speeds depend on what you're using, router or spindle. Make a lead in to your contour so the upcut entry is away from your finished edge to start. I have a PRT w/PC so I'd start at 1.5/sec and adjust on the fly from there.

I'm sure that marine ply will be tough on bits so keep the rpms somewhere where the bit doesn't get to hot and I like to use a shot of this stuff (http://www.hdlusa.com/catalog.cfm?ProductID=SADC11) between cuts too.

Scott

[edp]

Many thanks for the input on this job. The run is 54,000 feet so I really need to get the tooling and feed rates right. Once again, thanks for the input.

Ed

[dhunt]

Thanks for the tips.
This project to cut 1 mile+ of decorative facia board is due to start in a week's time,
consuming about 140 sheets of 1/2 inch marine ply.
Any more tips re. tooling and feed rates in the cutting of marine ply
would be v.welcome as we gear up for this run.
Thank you.

DH

[NSchlee (Unregistered Guest)]

David, Is this domestic (fir) marine ply? You might look into using 12mm BS1088 Okoume. This material is a higher quality than domestic marine ply. Much less chip out when cutting, no voids, no veneer joints, no patches (footballs).

Neal

[dhunt]

Unsure just what we will be supplied with.
Stock is yet to be trucked in from our local supplier,
but will be sure to let you know just what we get to work with, once it arrives.
Thanks for your interest: will keep you posted
most likely before the end of the week(?).

[gene_marshall]

have you thought about extira?

[elcruisr]

David,
If you want a good clean cut edge top and bottom try a compression spiral. I cut up thousands of parts in ply and I'm sold on Onsruds 60 series (and there are many other options out there as well). I use mostly 60-121 single flutes. You need the short upcut for 1/2" material. I can run at 8 to 10 inches a minute at 17,000 rpm with a spindle, don't know if you have a spindle or not. If your facia has alot of small details your feed speed will be slower no matter what you set and the speed will neet to be lowered to keep chipload correct.

Eric

[gerald_d]

Eric, is that 17 000 for a 1/4" or 3/8" bit? (I don't know the Onsrud numbers)

[richards]

3/8-inch

http://www.onsrud.com/Products.asp?Action=View&ID=1023

(It's an excellent cutter.)

[elcruisr]

Yup, 3/8". They have a 1/4" tool in the same series but you don't get as clean a cut because of a smaller gullet or so I'm told. In 1/2" ply I could run the 1/4" tool at 6 to 8 a sec easy and maybe 10 if the tool is good and sharp.

Eric

[edp]

The ply we will be using for the fretwork is a Brazilian marine ply, outer plies are amapa. The radii of all corners is 1/4" so we might be better off to use a 1/2" compression bit. The design is quite simple on the edge and has a plunged detail every 8" that is also simple with the same radii. Any thoughts as to whether or not the 1/2" bit might be a better choice?

[dhunt]

Thanks, Eric L., for your observations re. bits suitable for cutting ply.
So far we've always used AMANA bits but maybe we'll try something different,here.

No, we're not using a spindle,
we have a Porter Cable 3.5 hp. router running at a fixed rpm of around 16,000?
so we must think within this parameter.

Someone mentioned cutting speeds of over 1 inch per sec.
which seems a bit fast to me who usually cuts stuff at speeds under 1 in. per sec.
Can we really chew thru marine ply, at 0.25in. per pass (two passes)
at 1+ inches per sec.? - If so, I'm delighted!!
Please advise!
Thank you.

[jay]

David, I noticed in your post that you use Amana Bits. My wholesaler has just taken on the Amana line of bits but I have been reluctant to purchase any as I do not know anyone else using them.

Would you recommend them?

[dhunt]

In my limited experience with router bits they seem okay to me.
The Boss keeps me supplied with tungsten carbide spiral upcuts - v.tough bits -
and which give little trouble other than normal wear and tear down the slippery slope to Dullhood.
I hear him talking of ordering ONSRUD mentioned above, for this lengthy marine ply order,
and I'd happy to use something difrnt,particularly since the O-brand seems well liked.

But yes, AMANA is OK,
and I think the boss (who's been buying them for years) would say so too.

[elcruisr]

You should be cutting 1/2" marine ply alot faster than that and in one full pass at 16000 rpm. At least if it's an Alpha machine. If it's a PRT you might try it at 1.5 inches/sec. If it's an Alpha open 'er up and let 'er fly!

Either way with a compression spiral you'll have no trouble with a full 1/2" pass. You could use a 1/2" tool but they do cost more and unless you can move at Alpa feed speeds that 16,000 rpm number is going to mean shorter tooling life because of poor chiploading. It will, in theory, deliver an slightly better edge than even a 3/8" tool but I have found little difference in ply in the real world. Alot at that point depends on the core and with import ply you never know.

Eric

[bob_lofthouse]

David,

We only cut Okoume Ply in 6mm, 9mm and 12mm.

It's got a very nice surface.... But today whilst we were busy I went on the machine myself and cut thru at least 20 nails in as little as 5 sheets.

When bits are expensive you feel like crying. I have to pay the bills not the guys using the machine...

We have a 3hp spindle and use a 1/4 inch up and down spiral.

I can only dream of cutting our ply at Eric's speeds.

Eric,

Using a 3hp spindle and a 3/8ths up/down cut spiral what feed rate and RPM would you run 9mm Okoume at..... I know you may need more info but you knowledge is greatly appreciated and I really wish I could make it to your camp...

The machine is currently cutting between 50 to 80 8ft x 4ft sheets per day.

We are currently have our VFD set at 19000rpm and feed rates of 300ipm (12mm) in 2 passes. 360ipm (9mm) single pass and 480ipm (6mm)single pass.

[bob_lofthouse]

I just read my post..... and should really add that the nails were already hidden/buried in the Okoume Ply and not put in by us...

Just in case anyone thinks I completely useless... which I prob's am in anycase!

[elcruisr]

Robert,
I sometimes think the guys at the plywood mills like to throw us the occasional suprise. One started a fire on my vacuum table! My question is why would there be nails in plywood....... Maybe some scientists need to look into this!

About your 3 hp spindle, does it have ceramic bearings or steel? The upper limit for steel bearings, at least for colombo, is 18,000.

You should be able to single pass the 12 mm even with a 1/4" compression spiral. I've run single flute 1/4" tools in 12 mm at 8"/sec - single pass without breaking tools. Ditto for 9 mm and pushed 9.5"/sec in 6mm. Granted that was with very sharp tooling. If I'm using a tool all day I sometimes back off the feeds an inch or two a second or so the last few hours as the tools getting dull. Don't know if it is really needed but It's been quite a while since I broke a tool from feeding it too fast. At those speeds I'm usually turning 17,000 to 18,000 rpm and I fine tune by sound of the cut. If it's screaming less rpms if it's growling it's more.

That being said my tool of choice is usually a 3/8 diameter single flute compression cutter whenever possible. When you really start pushing a 1/4" tool hard enough you will get measurable deflection sometimes. In some parts this won't matter but for others it is!

Keep an eye on the bearing temps if you can, particularly the lower ones. 145F max under load. If you check them off and on during the day you will see the temp slowly rise as the tool gets dull. Over heating means you're past your loading limit for the spindle or it's time for a rebuild.

Eric

[dhunt]

Thought it might be nice for y'all to see what this was all about

4903

[dhunt]

-and another..
4904

[gerald_d]

David, there is amazingly little dust around. Was it all picked up by your collector, or did you do a little cleaning for the photo?

[dhunt]

Sorry, no intentional cleanup for Photo Op. purposes!
I continually cleanup, while cutting...
Our dust extractor system has an offshoot with a long extension hose,specifically for cleanup: I partially crack open its valve and busy myself, keeping it "down to a low roar",as they say..
Thanks for noticing!

[dhunt]

Gerald D...

speaking of dust collecting, I thought I'd post a pic of our dust collector.
In the foreground is our vacuum pump..
4905

[dhunt]

As we approach the end of this production run of marine ply 'gingerbread' facia board,
it turns out we cut most of it using a 1/2 inch-shank AMANA bit with two-sided replaceable blade inserts(changing out one blade per day)
at a fwd. speed of 1.2 inches per sec. on our (non-Alpha) PRT96 ShopBot,
averaging about 8 sheets of ply per day, which yields 40 eight-foot strips.
- not bad fer a buncha West Indians...

[dhunt]

A final photo related to this thread, showing a stack of about 50 sheets of 1/2 inch ply waiting their turn to be cut into strips of facia..
Apologies for the cleanliness of our ShopBot room,
but it wasn't done expressly for photo purposes, it's just the way I run the place, constantly vacuuming the floor
4906

[jhicks]

I am constantly struggling with the feed and speed subject but generally run at between 1.8 and 2.0 IPS on Trupan, Poplar, and plastics we cut at between 14,000 and 16,000RPM on a 5HP spindle PRT120 at 1/4" depth per pass or the OD of the bit as a guide. Usually a 2 flute or O flute bit is what we find delivers the best edge result and mimimum chatter. What I never have figured out is the debate over speed between an Alpha the PRT and other brands.
If the chipload/bit combination dictates speed and feed, how does one get to these "high move speeds" above 3 IPS/180FPM without overload, breakage, and overheating?
I have occasionally dialed up to 2.5IPS with 1/4" depth of cuts but still am perplexed about higher move speeds related to proper chip load?
When I consulted with Onsrud, they seem to slow me down further as I increase the depth for single path cuts 1/2" or 3/4" so I just end up making multiples anyway.
Can anyone clarify this? How does one achieve these "Lightning move speeds"? Is the 12 IPS just a move between points advantage or is it really a cutting/move speed?

[elcruisr]

When I run the prt with a single flute 3/8 compression on something like trupan I will typically run at 1.8"/sec and 11 to 12,000 rpm. When I run the same tool on my alpha I run at 10"/sec at 17 to 18,000 rpm. The rpm variance depends on how sharp the tool is. Both machines have 5 hp spindles and I cut full single passes in 3/4" stock. Remember that chipload specs are an approx. guideline, not cast in cement! The real issues are edge quality and tooling life which will usually be achieved in a chipload range not a specific point. Different cutter, machine, edge quality and material combinations will require different approaches.

[jhicks]

Thanks Eric. Wouldn't that scenario allow you to change the PRT to its fastest practical move speed and adjust spindle RPM's up? I understand the load calculator is an approximate but by using that same base line as a starting point,
My chipload calculator says your 1.8" at 12,000 =.018 which is about the same with the 2.2"/sec at 14,000rpm.
Guess I'm just confused with why one would move at 1.8" when 2.2 could be the rate?
My chip load calculator doesn't go higher than 4.0 feed rate but it says at 18,000 rpm to achieve the same load on a 2 flute cutter of .018 the move speed would be 2.7"/sec not 10"? Thats a pretty big leap.

Please help me understand what I'm missing about greatly increased Alpha speeds. Is a different chipload calculation somehow involved.
By the way does shopbot have a new download on the chip calculator that reflects these higher Alpha speed rates?
The one I downloaded is ChiploadCalculator-3483[1]\RPM Chipload Calculator.exe"

[Brady Watson]

Jerry,
You might have missed the part about Eric using a SINGLE flute tool. Using the calculator, you would get a chipload of .03" for a single flute tool @ 18,000 RPM & 10 IPS. This is a pretty heavy load, but not too large for a 5HP spindle to keep up with.

Like Eric said, "Different cutter, machine, edge quality and material combinations will require different approaches." and "Remember that chipload specs are an approx. guideline, not cast in cement! The real issues are edge quality and tooling life ..."

The BEST way to get the 'right' chipload is to go out and cut, while keeping a log of what parameters you used. Since only YOU can determine what is an acceptable cutting time and edge quality, the chipload calculator can't take that into effect. By going out an cutting using different settings/speeds etc, you will quickly understand how to determine chipload without using a calculator. I have never used a chipload calculator...Here's my way of determining chipload for the types of things that I cut (just about everything):

1) Does the edge look clean?
2) Am I pulling off nice big chips without bogging down the router?
3) Do I smell burning?
4) Does it sound 'right' when I am cutting?
5) Is my bit sharp?

These are the questions that run thru my head when trying to determine the right speed for a given job. In some cases, mainly when cutting plastics, it makes a big difference when you do a few passes with let's say .02" allowance left on the part and a bottom skin (don't cut all the way thru) and then go back and finish the cut with no allowance and full depth. This gives you a nice clean edge, no step-down marks and keeps the tool moving. If you go too slowly in plastics, they often work harden and become brittle...and are even more of a challenge to cut.

Eric is able to cut at the speeds he does because he has done the research, testing, tweaking and is most likely using a cutter that is designed for a particular material thickness.

-Brady

[elcruisr]

Brady's right. I use a tool that I've been using for over four years and have it pretty well dialed in for what I do and the edge quality that my customers are happy with. The PRT could run at maybe another .2" a second or so but I tend to run very non critical jobs (time wise) on it and don't want to take the chance of missed steps. There was a day I pushed the PRT for all it was worth but now the Alpha covers those jobs. Don't get too hung up on the perfect chip load. Like Brady says, cut material, keep a log and you'll start to figure it out.

Eric

[jhicks]

Thanks, I'll keep playing but am still amazed at the ability to go from 2"/s to 10"/s with such deep cuts. Guess I'll need to get more agressive and do some more testing to max it out.
What exactly is it about the Alpha that allows one to make such a substantial leap? Obviously the bits will hold up so is it all in the steppers and software keeping up with the mechanics?