Smooth Cuts in Hardwood?

[Lee Miller]

I hope I'm not already in danger of wearing out my welcome, but I have a question about cut quality in hardwoods. Until today, I've been practicing on various grades of Pine and found a better cut is made in the better grade of Pine. I cut some Cherry this afternoon and got a really rough cut. I hope it's not related to cutting into a hold-down bolt the other day.

Can someone point me in the right direction to start getting up to speed on the factors related to smooth cuts in various woods?

Lee

[steve_g]

Lee…
What I’m seeing… The watermarks of your three step-downs tells me you’re not cutting with an onion skin strategy.You should cut in climb mode with a .01”-.015” allowance away from your perimeter vector, and then make a final pass, full depth, in the conventional direction, on the line.
This should help… as will not cutting into hold down bolts! J
SG

[barrowj]

Lee,

I've cut quite a bit of hardwood, including cherry and have not seen that bad of a problem. A number of factors could be hurting you but will need more information. 1st, cutting into your hold down bolts may have damaged your bit enough to cause this (trust me we have all done that) and we would need your feed rates ( x, y, z). This will help us to see what may be contributing to your problem. Of course Steve has a very good suggestion and I have read this several times on this forum and must admit I keep forgetting to follow it myself.

Joe

[Brady Watson]

First, check your Z axis to make sure it is truly perpendicular to the table. I see waterline marks & when I see that the first thing to check is router squareness.

Second, analyze the scrap pieces in comparison to the finished parts. Does the scrap look better? "Don't throw away your best edge." - If it does, reverse cutting direction. If running Climb, change to Conventional in the profile toolpath strategy fill-in sheet - right under where you selected the tool bit - or vice versa.

Third, experiment with higher RPM. Try running somewhere in the 1.5 to 2 inches per second on the XY and 1 in/sec on the Z. Set your RPM somewhere in the 13,000-15,000 range. See if the cuts improve. Focus on getting the best cut quality. Softer woods require higher RPM. These are just baseline numbers. adjust one or the other until the cut quality is improved.

Pine is junk & not easy to get a clean edge all the way around. You need good fresh tooling to get your best edge. You should be running a 2-flute upcut spiral (or solid carbide end mill) or straight bit for this job.

Try it out and let us know how you make out.

-B

[gary_n]

Brady,

On a 2001 PRT, with a spindle, would there be enough adjustment in the v-rollers of the Z axis, to adjust this problem? You can't access the screws for the spindle mounting to make the adjustment without completely removing the Z axis. If there is another way, please advise. Thanks in advance.

[maverickx50]

here is a nice article about cutter feed speed etc.

http://makezine.com/magazine/cnc-routing-basics-toolpaths-and-feeds-n-speeds/

[Brady Watson]

Brady,

On a 2001 PRT, with a spindle, would there be enough adjustment in the v-rollers of the Z axis, to adjust this problem? You can't access the screws for the spindle mounting to make the adjustment without completely removing the Z axis. If there is another way, please advise. Thanks in advance.

The adjustment is entirely with the 1/2" bolts that go through the 2x2 'towers'....OR clocking the spindle plate a little bit. Get a good square and see where it is...Dial indicator is the preferred method.

-B

[dlcw]

I cut hardwood all the time and use the method Steve G recommends. I also use this method for cutting plywood. Very clean cuts perfectly on the line.

The Shopbot has enough slop in it that trying to cut everything conventional leaves less then desirable results. The climb then conventional method removes this and provides for excellent results. The down side is it takes longer to cut everything. But that's life. If you want super cuts on single passes you will probably need to go with a big-iron machine that is much more rigid.

[Brady Watson]

The Shopbot has enough slop in it that trying to cut everything conventional leaves less then desirable results. The climb then conventional method removes this and provides for excellent results. The down side is it takes longer to cut everything. But that's life.

Don - I don't agree with any of these statements. I certainly don't get cuts like that on my machine and only do climb with allowance, then conventional, for acrylics where the edge quality is critical. If I had to go through that nonsense on every job, I would have ditched my machine long ago and bought something else.

The reason machines 'have slop' in them is because they have not been properly maintained or they are being run 'chipload heavy'. People start to get Scotch with their carbide and run them at 8,000 RPM. That's milling machine territory & not routing territory. Running the same chiploads as heavy iron is going to result in poor cuts on these machines. You can't make any money if you have to do the climb/conventional trick on every job...and you certainly can't send out parts with waterline marks on them - at least I can't/don't.

-B

[scottp55]

Also, Lee has a 2 week old Desktop.
Should be just a feed/speed/damaged bit issue.

[curtiss]

Could someone briefly explain when it is best to use climb/conventional ?? With an upcut everything becomes the opposite correct ??

Still confused, thanks

[Brady Watson]

Conventional is the "conventional" way of using a hand router. Counterclockwise on outside profile cuts; clockwise on inside cuts. Climb is just the opposite. Climb, 'climbs' on the material pushing the fibers in. You cannot do this by hand because the router will want to run away from you & out of your hands.

This has nothing to do with the bit.

-B

[Lee Miller]

Thanks everyone. As Scott mentioned, I've only had the Desktop for eight days. Today is the third full day I've had to work with it. My "real job" is seriously interfering with my time in the shop.

I used the 1/2" straight bit when I was surfacing the spoilboard and hit the hold-down bolt. It just clipped the edge of the bolt and spun it out of the board with minimal damage to it or the bit. The bit is still good for surfacing as the damage is half way up one cutting edge. I haven't used it for anything else.

I've been using the 1/4" down-cut spiral that came with the starter kit for all other cuts. So far, I've only used the default settings for the tool.

I checked the spindle alignment and, as far as I can tell, it is perfectly square to the newly surfaced spoilboard.



I've spent a few evenings looking over the sample part files and the part files a few of you have shared with me. I've read everything I can find on the OpenSBP COMMAND Language, and I think I have the basics down - at least I can read a program file now and understand what it's supposed to be doing.

So, with all your sage advice and a lot of reading, I think I'm ready to start experimenting with speeds and rates and toolpaths.

One other thing I need to improve is my hold-down method. I'm using screws and I predrilled the material, but not the spoilboard, so I thinks there may have been some movement. Also, I'll add double-sided tape.

Any thoughts on "up-cut" vs. "down-cut" in hardwood? Does "up-cut" apply any downward pressure on the material to help with the hold-down method I'm using?

Thanks again for all your advice. You guys are awesome.

Lee

[Brady Watson]

An upcut will evacuate the chips from the kerf, but will fight your hold down effort. Read this (http://www.shopbotblog.com/2007/03/a-tale-of-three-bits%E2%80%A6and-the-poor-man%E2%80%99s-compression-spiral-trick/) real quick to get a little bit of clarity about up/down/compression.

Since you are working on a DT, you may want to add carpet tape to your bag of hold down tricks. Read this. (http://www.shopbotblog.com/2006/03/a-sticky-situation/)

Experiment with a combination of screws or tape and tabs/bridges via the profile toolpath options in the toolpath fill in sheet in VCP. When it comes to machining, figuring out a good hold down strategy is like 80% of the job...so don't fret.

-B

[Joe Porter]

Lee, I either use a good quality carpet tape or screws for hold down. For screws, I use the pocket screws (Kreg) with about a half inch protrusion and a fine thread and a lite touch on the power screw driver. You can always pull them tighter by hand. I do pre-drill the work, and maybe a little into the spoilboard with a properly sized drill. Once you have the screws, drill and driver all set up, this becomes an easy and quick method of hold down. Don't use too big of a drill or you may have a little movement in the material. As far as not hitting your screws, place them in the drawing in your design software (V-Carve) with an accurate measurement and transfer this to your material and be accurate with your material size and alignment as far as your zeroing X and Y. Hope this helps...joe

[Lee Miller]

Thanks Joe. I went to ACE Hardware yesterday and bought some of their heavy duty, indoor/outdoor carpet tape that Brady recommended. Before that, I used some double-sided tape I had on hand which turned out to be a nightmare to clean up. I don't remember what type/brand it is but it's definitely too strong and messy for this application. I'll try the carpet tape today.

I really like your idea to include the screw placement in the design drawing. I think the limited work area of the Desktop makes the screw/tape method my best option for hold-down.

[Lee Miller]

Success!

After much frustration I am finally getting relatively smooth cuts in Cherry and Walnut. The down side is I don't know what I was doing wrong to begin with. I fiddled around with feed rates, RPMs, ramping, Conventional/Climb cuts, tape and tabs, etc., without much improvement. I tried a straight bit and the striations went away, but when I tried an up-cut bit with the default settings, the cuts were way better - no chatter, no striations, and super quiet.

Could it be that the down-cut bit is flawed? I didn't hit anything with it and looking at my original cuts in Pine I see the same issues, they're just not as noticeable because the Pine cuts were pretty rough anyway.

Oh, and I did have one mishap. I was cutting a profile cut in Cherry with the down-cut bit and on the second pass it did a lot of stuttering and offset the whole cut an inch and a half. I had to re-zero everything, of course. Not until the next attempt did I realize that when I warmed up the spindle I forgot to increase the speed from F100 to F200 and the RPMs were way too low on the previous cut - I assume that's what caused the problem. I'm confused by this as I thought the spindle speed was controlled by the cut file and not the VFD.

Anyway, I am able to get production back on and I'm happy about that.

Thanks again!

Lee

[Brady Watson]

Spindle RPM is NOT controlled by SB3 on a Desktop machine. The VFD doesn't have provisions for external control.

Yes...running at 6000 RPM will do it!

Keep learning - and more importantly, observing.

-B

[scottp55]

Lee, The bigger machines set their speed in the program, we have to do it manually.
If you look at #9 on this thread, Ryan explains it.
http://www.talkshopbot.com/forum/showthread.php?18632-Spindle-speeds-automatic&highlight=desktop+spindle+speed

I think it may have been a combination of a lot of things. I almost Never go below 9,000 rpm(2 bits/special need/slow feed).
Including the Desktop VFD vs RPM chart with the warm-up routine at the bottom...Do they have a new one?

Glad you got going, but surprised it was with the default settings in hardwood.
Going to have to try them again in scrap to remember why I don't use them:(
scott