Simple v carving shows problems

[Chuck Keysor]

Hello everyone:

I have cut a very straight forward plaque as part of learning how to run my PRT alpha 60 x 144, with 5HP Columbo spindle, a brand new 1" 90 degree V-bit into a 1/2 inch thick piece of PVC that is 6" x 19". The spindle was running at 13,000 RPM, and the cutting speed was 3 inches per second. The stock was nailed to the spoil board in 6 places. The spoilboard was recently flattened, after having trued up the spindle by methods outlined on this forum.

My cutting results were rather disappointing. The bottoms of most letters were poorly defined. There was a lot of chattering along the side walls of most letters. Please see the two attached photographs to see the problems, and some added information. Note, I used a stiff toothbrush to clean out all the grooves, so all the debris you see is actually stuck on.

It is of note, that along the long straight border, the v-groove had a sharp v groove bottom, unlike the letters. And the boarder's side walls are also free of chatter. And some parts of some letters have very little chatter on their sidewalls.

I layed out the text in Adobe Illustrator, and imported it into Aspire. After looking at the carved results, and trying to compare the Aspire vectors, I didn't really see any correlation between the nodes of the vectors and any of the chatter on the side walls.

I did cut some similarly simple plaques before Christmas, made out of oak. My results were similarly disappointing. They took a lot of cleaning up to make them presentable. This PVC plaque will also require lots of manual clean-up (and Mother's day is almost here...).

I suspect that this is a dynamic/motion issue, where the system is going into undamped vibrational modes when the chatter occurs. The simplest thing to do that I can guess at, would be to try and cut this at a very slow speed, but that wouldn't really fix anything. And even at 3IPS, it took about 20 minutes to cut this simple plaque. And, I don't have any more of this material left to make another test cut at a slower speed.

What should I do to improve the quality of my V-carving? Thank you very sincerely, Chuck PS: Sorry in advance for this being another long post....

[CNYDWW]

It sounds like your V rollers on the Z axis aren't tightened properly. With my PRT it's a bit of a pain to loosen the bolts just enough so you can get a good feel of when the bearing is engaged on the rail or not. If the groove in the upper part of the first photo is along your X axis. It would also support my theory. First few times i've tuned my router plumb, it's been a bear making sure the V rollers are just right.

Regards
Randy

[Chuck Keysor]

Thanks Randy. The long groove/border at the top of one photo, and along the top and bottom of the other photo, is parallel to the X axis. IE, the text, runs left to right parallel to the X axis. Chuck

[Mayo]

Maybe it's the Z rollers, or the material moving, or the cutting speed could have been too fast and resulted in chunks being pulled out rather than slices being cut off. Or some of all of the above. Or maybe the bit isn't really all that sharp even if it's new.

If the sign is still attached to your spoil board, try cutting it slower and just a fraction deeper. Some of the serifs may blend together if you cut deeper but if you're not happy with it anyways...
hand carving it to clean it up will be an exercise in patience if nothing else.

Or you could resurface the PVC, flip it over, and cut the sign again on the other side.

I'd stop over to check it out but this week I'm dog sitting and don't feel good leaving the guest dog alone with my dog. Next week or maybe this weekend Saturday or Sunday I could stop by and then two of us can both get bewildered! I can even bring over a couple discs of HDPE or some other scrap stuff.

[myxpykalix]

Chuck looking at the picture is that your final cut with all the shavings swept out? If so, have you checked the 1) the bearings in the spindle 2) the spindle in its cradle to see if it is tight 3)the router bit itself ?

It seems to me that your outlines of the vertical lettering is for the most part ok, that says to me that it might not be your v rollers.

If you have this same issue with other material then you can rule out the material. Where you are having the issue is in the confines of the letters and that suggests to me that it is with your spindle or bit. Is your spindle tight and not vibrating?

can you perform some tests? Do you have a different 90 vbit? Try making some lines both vertical and horizontal with different vbits at different depths. That is at least one way to rule out the bits.

[Chuck Keysor]

Thanks for the replies. Sorry it took me so long. I spent over 2 hours touching up the v-carved grooves with some chisels and knives. I only made the plaque look less bad. But I figured a generous dousing of black paint would go a long way to hide the flaws in the grooves. However, I did manage to get this into the mail this afternoon, and it should get to my Mom before Mother's Day.

Randy: I will check my V-rollers on the spindle carriage. I will use the assembly manual for my reference. If that doesn't help, I will do a forum search. Certainly others have had this same problem before and gotten good tips.

Mayo: It would be GREAT if you could come over, wheneverit works for you. Before you come, I will make some test cuts in the left-over piece of PVC I have. As to chunks being pulled out, as I spent my time cleaning up this mess, it seems as though the crud on the bottom of the grooves was really stuck on, so it may have been remelted PVC. I will try the bit I used, and the couple of other 90 degree bits as well, one of which is also brand new and never been used.

But before I read your post, I had already taken the plaque off of the machine to do my manual touch-up. However, in retrospect, re-running the file, would have probably been the way to go (instead of chisels and knives).

I will also make another plaque using the same cut file, except this time it will be made of oak. At least I can eliminate the possibility that the crud on the bottom of the grooves was remelt.

Again Mayo, I am thankful that you can come at some time to help me get a handle on this.

Jack: Yes, what you saw was the final cut with everything loose removed. I have not checked the spindle bearings. Having never heard anybody else's spindle, I can't say I know what one should sound like. But mine seems pretty quiet, and I have heard bad bearings in other motors over the years. And after the spindle had warmed up, I did tweak the RPMS around, looking for a point where the machine sounded quietest. (Though for all I know the sweet spindle speed without any cutting load, goes out the window when the cutter is actually engaged.) I will recheck the spindle attachment to its mounting plate. I can't say as I have checked it since I re-squared my spindle for resurfacing my table top with that new 2 1/2" Amana surfacing bit. (By the way, based on earlier posts, the fact that with such a big bit, my spoil board turned out so well, should at least show my Z axis is squared up in both directions.) And, I will try and see if the spindle itself seems to be vibrating. As to test cuts and other bits, I will do that, as requested previously.

Barring un-forseen issues, I will make a check list and try each suggestion, and then report back.

Thank you all again, Chuck

[Chuck Keysor]

A quick note. I just got done cutting the exact same file in MDF. While the plaque was being cut, I changed the spindle speed, from a high of 14,000rmp, down to 8,000rpm. I made marks of the speed on the board so I could look for the effect of the RPMs on any of my previous problems.

1) The bottoms of all the grooves turned out very clean and sharp, no matter what the RPM settings were. So all the garbage on the bottoms of my grooves cut in the PVC were in fact re-melted pvc.

2) The chattering on the sides of the letters was almost entirely gone when the plaque was cut in MDF. I used the same bit (I didn't touch it in any way from the previous cut in PVC) and the same 3inches per second feed rate. And I attached the plaque to the spoilboard with the same amount of nails.

3) I am making a test file for the PVC, and will vary the RPM settings as I go to see if that helps my remelt problem. I'll post pictures of the new PVC and MDF tests later today.

Chuck

[zeykr]

PVC you need to spin slow and move fast. Bit geometry can make a big difference also, a bit that cuts wood well may not be the best choice for pvc.

[Chuck Keysor]

I recut the original file, using the same bit, but this time in MDF. I then l looked for the worst letters from the original PVC plaque, and made a new cut file using just the worst letters to cut the PVC.

As I ran each plaque, I adjusted the spindle RPMs from 8K up to 14K. I scribbled the RPMs onto each plaque as it was cutting.

For the MDF, most of the chatter on the sidewalls was gone, though there were still some traces, and those are shown in the second attachement. As I study the board, I can't see any difference in the cut quality over the 8K to 14Krpm range. And as noted previously, the bottoms of the grooves are all very clean, so the first PVC plaque was messed up from re-melting of the PVC. And, the V-bit I am using, does not have a sharp point, (as described in a post several days ago). Its minimum line cut width is .02" which keeps the very bottom of the grooves, and the little end of letter details from being really fine.

The new test plaque cut in PVC turned out very badly. There was tons of remelt, . And, I can't see any difference when changing the RPM from 8K to 14K. There is still some chatter on the sidewalls, but it also seems less this time. The piece of PVC was cut off from my earlier plaque, so that is not an issue. And I attached this to the spoil board the same way as before, with small nails, and it was really on tight.

Ken, I had my speed set in Aspire, for 3IPS. I don't know how to change the cut speed/IPS dynamically. I actually only know how to change it in Aspire, which shows how little I know about my Shopbot interface.

But Ken, do you have any recommendations as to how fast (IPMs) I should be running? And what RPMs, (assuming if the IPMs get into a good range, that the RPMs would have an effect) would you recommend?

The V-bit I used was MLCS part number 7729. Do you (or anyone else) have a bit you would recommend for V-carving PVC? (In an early post, I was told by experts to stick to Onsrud, Amana, etc. which I haven't purchased yet, so your recommendation will be timely.)

Jack, I really couldn't tell anything about my bearings. The spindle seems really tightly attached, and I tried to feel the body for any unusual vibrational modes while my test plaques were being cut. But I didn't notice anything.

Randy, I haven't tried to mess around with the V-bearings yet. I was hoping for some other feedback before I toss another big variable into the mix. But that will be the next thing I try, unless someone else suggests some other tests first.

Thanks, Chuck

[jim_vv]

Greetings, Chuck

I have not V Carved PVC so I may be wrong here. . . . I may have missed it, but have you tried slowing your move speed down? I have a PRS Alpha which will move fast like your machine. I think that 3 IPS may be too fast for V Carving. I have great success in V Carving MDF, soft woods, and hard woods at 1.33 - 1.67 IPS. I use Onsrud 30, 60, 90, and 120 degree cutters. I run the 2 edge cutters at 14K-15K RPM and the 1 edge cutters at 18K RPM. For V cutters, Onsrud's chip loads are the same for plastic and wood. For 2 edge V Bits Onsrud recommends a .001"-.003" chip load. For 1 edge Engraving bits they recommend a .004"-.006" chip load.

If you have the material, try running at 1.5-1.67 IPS, .5 Plunge, and 12K-15K RPM.

Let us know how it goes.

Kind regards,

JIM

[jim_vv]

Greetings, Chuck

You got me thinking about V Carving PVC so I did a little testing this morning. I think that your text is too small for a 90 degree V bit. Additionally, my machine would shudder quite a bit if I were V carving such small letters at 3 IPS. V Carving creates a lot of moves all at once.

For my test I V Carved .55" tall letters (Engraver font) with a 1" 60V, a .75" 90V, and a .25" 60V engraving bit in a scrap piece 0f 1/2" Sintra. I held the sample piece with carpet tape. I ran the 2 FL 60V and 90V cutters at 1.5 IPS and 15K RPM. I ran the 1 FL 60V Engraver at 1.33 IPS and 18K RPM. After blowing out the chips I decided to run a second pass which helped quite a bit. The 2 Edge 90V yielded the poorest result and the 2 Edge 60V yielded the best. Perhaps when I have more time I may do some further testing to get V Carving PVC really dialed in. My cutters are from Onsrud, but I do plan on trying Centurion when I need to purchase more. Also, rather than nailing your work down, I would suggest that you use screws, clamps or double sided tape for hold down (assuming you don't have vacuum).

I have attached some pictures of my test piece.

Kind regards,

JIM

[paulkiecka]

...Ken, I had my speed set in Aspire, for 3IPS. I don't know how to change the cut speed/IPS dynamically. I actually only know how to change it in Aspire, which shows how little I know about my Shopbot interface.


Chuck to change IPS while your file is running, use Shift < and Shift >

when cutting I was an engraver/signmaker years back, I would use either half round or quarter round bits with one cutting edge.

[Chuck Keysor]

Jim, thanks for your awesome reply! Everything you said makes sense. The shuddering of my machine had me worried, and I had of course assumed something was out of whack. Having a wrong premise can derail clear thinking. But your clearly documented test cuts is greatly appreciated (by me, of course, but certainly others as well).

I noticed in my lengthy post, that I failed to say what size my letters are. My letters are 9/16" for the capitals, and 3/8" for the lower case letters, so your guess was pretty good.

I will try re-running at slower IPS, but will have to resurface the one piece of stock I have.

I do have 45 degree and a 60 degree V cutting bits, but I didn't want to use them, because brand new, I found out that their points are not sharp at all. So I chose the 90 degree bit because it had a much sharper point.

You said you ran one pass, and then went back and ran another pass. On your second pass, I am assuming you did not take a deeper cut, but in essence, the repeat pass just cleared out all the gunk that shouldn't have been there if the first past went perfectly. Is that correct?

Do you use Aspire? It allows (as I read the control panel) multiple passes. You declare the depth per pass, and when so doing, you specify the clearance path step-over, and the final pass step over. What values would you recommend for V-Carving?

Oddly enough, I have a 6 zone vacuum table, with a HUGE Roots "blower". However, I have not actually fired it up. I bought it used, and the limited instructions said to be sure to check oil level, and check for rust if the machine has been sitting unused. I don't know how to do either, and have failed to investigate, so it just sits. (Perhaps subconsciously I am avoiding the noise, heat and big electrical bills.) It seemed as though the finishing nails would cause the least damage to my spoil-board.

I see you are not far from Wilmore, KY, where I lived for the last two years of High school (Jessamine County High), before I went off the the University of Kentucky. I have a fond spot in my heart for the Bluegrass, though I would not have admitted it back in the 1970s.

Paul, thank you for telling me how to change the IPS settings while my file is cutting!

Tomorrow, I'll try cutting at varying speeds, and I'll try my 45 and 60 degree bits.

Thanks, Chuck

[steve_g]

Chuck

I want to point out some things about speed changes...
As has been pointed out here several times [shift]+[>] or [shift]+[<] should be reserved for fine tuning as ramping is not recalculated unless you pause and resume... It is VERY easy to edit your .sbp file. Open it with any word processor, MS "word pad" or best of all... in SB3 ---> file ---> Part file edit. The MS command determines Move Speed by using the parameters following it... See the attached photo for just exactly what you will see. Change the parameters, save the file and run it.

Try it... you'll like it!

Steve

[jim_vv]

Greetings, Chuck

I have gleaned much from this forum so it is a pleasure to be of assistance when I can. If you are ever in the area do let me know so that we may meet.
I use ArtCAM Pro.
I have attached screen shots of my 60V and 90V settings. I would run the 45V at the same FR and PR.
The "second pass" was just me running the same file over again which cleaned out whatever didn't come out with my blow gun.
I don't think that the lack of "point" on your cutters will be an issue.

Let us know how it goes.

Kind regards,

JIM

[Chuck Keysor]

Steve, thanks for the information on the command information on IPS changes in the SB file. I used the SB editor to make the change. Thanks again.

Jim, thanks for the added information.

The PVC tests I ran Monday were only conducted with a 90 degree bit. I have attached three photos of the PVC: an over-all shot of one side all cuts made at 1.5IPS but various numbers of passes (the flip side used the same file, but cut all in one pass at 3IPS). Then there are two detail shots, where I put different views right next to each other.

PVC/Remelt: Multiple passes worked very clearly in cleaning up the long swoop/swoosh providing good results (ie, the remelt was all removed). But with the letters, multiple passes only made bad less bad. I even did three passes over some of the letters, and the third pass had only a marginal effect, if any. So right now, I can not carve letters in PVC acceptably with a 90 degree V bit (but I can in MDF).

PVC/Jitter/Chatter: With PVC, the bit jitter/chatter really only showed up on the "swoosh". Capturing the jitter/chatter on "film" is rather difficult. The second attachment shows MAYBE a little less chatter at the 1.5IPS setting (which also had two passes). I don't know if I am hoping for perfection that is not attainable, or if there is reasonable room to obtain improvement. And if there is room for improvement, is it obtained by changing other mechanics of the system..... Comments, suggestions???

MDF/Jitter/Chatter: I tried capturing chatter in MDF, but my tests there were confusing (I altered too many variables at once), so I haven't posted those results. But it did appear as though the chatter was reduced or eliminated where I could make corrolating comparisions. So I will go back and go back and run more focused tests to directly compare the effects of IPS reduction on the reduction of bit chatter.

Chuck

[Brady Watson]

Chuck,
I never v-carve faster than 1.5,0.7 IPS as the quality of cut will suffer. Aside from the tool being thrown all over the place with 3-axis moves, the v-bit by nature does not cut at the very center of the bit...so it winds up dragging across the material, as can be shown in your 3 IPS vs 1.5 IPS pics above.

For these smaller letters, I would pull the speed down to 1,0.5 IPS and then note the quality - which is what should be the focus, not speed. It is physically impossible for your tool to go 3 IPS at ANY point on those little letters - which means that there are certain cases where ramping is triggered at a point it may result in jerky motion.

Slow things down & I think many of the quality issues you are having will go away.

-B

[jim_vv]

Greetings, Chuck

As I said before, I would suggest a 60V for your small letters. At this size my results with the 90V were the same as yours. You are welcome to come down and borrow one of my 60Vs. :)

JIM

[Chuck Keysor]

Thank you Brady and Jim for your helpful replies.

Brady, I will pull my cut speeds down for my next PVC trial. In connection with my quality issues, I had recently posted questions about problems I was having with some very fine lined woodcut images, and those too were run at 3IPS x/y so now I also have to go back and try those at lower IPS values. Hopefully with better bits, and the slower IPS, I will manage to get better results.

Jim, thanks for the offer of the V-bit. Last time I was in Kentucky, was more than 20 years ago, so I don't expect to bump into you any time soon. As to the 60 degree bit, as I had run out of PVC, I did run a series of other V-carving tests in MDF. I cut a series of letters, from .625" high, all the way down to .15" high. Without any exception, the finest results produced were with the Amana 60 degree cutter (part of a set of sign cutting bits with replaceable cutters.)

I think I will take a further step backwards and do my experimenting on V-carving using MDF, and wood. The PVC has introduced too many problems. After I get the MDF and wood carving down, I can move back to PVC. I do have a need to cut PVC, so that is why I chose that for testing, not expecting it would introduce its own problems.

Thanks Brady and Jim! Chuck

[Chuck Keysor]

As a general question, if anyone else is still following this thread, I do need to buy more cutting bits for practicing V-carving. I have MLCS 45 degree, 60 and 90 degree v-bits, and 30 and 60 degree bits as part of the above mentioned Amana interchangeable cutter set.

Two of the first brand had real issues. And one of the 30 degree interchangeable bits had its tip break off the very first time I used it when it was cutting MDF, at 3IPS, and the depth of cut was not more than .2". So I was disappointed there. I need some good bits and I want to try some other brands, and Onsrud seems to be very highly recommended.

My question is, is there someone who sells sets of Onsrud v-carving bits at a good price? I did some poking around on the Internet, and I don't know how to tell who is a good provider and who isn't, and who makes good deals.

What I'd like to have a full range of two (or three?) bladed V-bits from 30 degrees to 90 degrees, all from one company (Onsrud), and of course I want bits that are good.

Can anyone make some positive recommendations? If such promotional things shouldn't be promoted on the forum, you can send me emails at chuck.keysor@sbcglobal.net

Thanks, Chuck

[Bob Eustace]

Hi Chuck

In hardwood you just cant go past the Onsrud 60 and it does have an exceptionally sharp point. In softwood we use 90 degree - 3/4 from would you believe Rockler. We get them when on specal at under $15. We are fans of the second pass technique as Chrissy hates sanding! We engrave a lot of acryllic too with the Rocklers. Rather oddly we get the worst results from Centurian solid carbide with the one edge. (fuzzies).

We need feed higher than 1.5 ips on softwood and 1.0 ips on hardwood.


Bob

[Chuck Keysor]

Jim, thanks again for your input, and especially the exceptionally clear, well prepared photos showing the results you got with each bit. What particularly caught my attention was the difference in the two blade v-bits versus the single blade bit. That reminded me of improved cutting I had experienced with a three blade flush trim bit, versus a two blade flush trim bit. And it also prevented me from going out and buying a set of those single blade V bits, as I had previously considered.

I went back to read old postings on V-bit recommendations, and found several for CMT Laser Point 60 degree bits. When I looked at the spec sheet for that bit, I saw it has 3 cutting blades. So I ordered two without hesitation. So even though I did not purchase what you use, your post was very key in my buying decision.

When I get my new bits, I will run some test cuts, at 1.5IPS and post the results. Thank you again, I really appreciate you input, and that of all the other posters. Chuck

[steve_g]

I'll bet on it that you fall in love with the three flute CMT laser point bits!

SG

[Chuck Keysor]

I got a pair of CMT laser 60 degree v bits, and cut a plaque at 10KRPM and 1IPS. I was a bit reluctant to post this result, since I had cut this in oak, some of the letters are 7/8" high, others are only 3/8" high and my earlier tests were in mdf and PVC with .5" high letters. But even though these changes perhaps invalidate a scientifice comparison, I was very happy with the results. There was only a very small amount of chatter on the letter o, but they look worse in the photo than in real life.

A few notes/questions:
a) CMT only seems to make their laser tip v bit in a 60 degree version. Isn't that strange, as I would also like to be able to get this quality in a 90 degree and 45 degree version as well. Did I just miss these models in their catalog?
b) The dark staining at the bottom of this plaque is actually from nails that had been embedded in the wood. A single nail, produced an indigo blue stain, perhaps as large as a football, and the fringe of that discoloration is at the bottom of this plaque.
c) I had varnished the blank, and then wiped on black oil based paint. The only drawback was some loss in the sharpness at the bottom of the v carving. I tried using a black/Jacobian stain, but that just wasn't black enough. Others have recommended black spray on ink when using a mask. Does spray on ink dry super fast, like spray paint? If so, I wouldn't want to use it, as even using latex black paint was terrible (on a different plaque) as it would not all wipe off, and required lots of sanding to clean up).
d) Is there any reasonable good gold paint that I could use for the gold rings? I tried two types of gold paint, one was terrible, and I had to remove it, and the other was marginally acceptable. (I suppose gold leaf would have been great, but I am cheap, and am giving this plaque to a friend who will be happy with the murky gold paint!)

Thanks, your advice has certainly improved my V-carving! Chuck

[steve_g]

Chuck

Nice work! looks like you've got your issues sorted out.
I've never seen the laser point 3 flute bit in any thing other than 60°. I even checked the CMT web site... no 45 or 90s available. it's a shame...

SG

[adrianm]

I love my CMT laser bit. Fortunately I managed to find a local supplier that does a bit that is near enough as makes no difference the same and comes in 60 and 90 degrees, 1/2" and 1/4" shaft and different diameters.

Unfortunately they don't ship to the USA. They list them as engraving cutters so perhaps searching for those might yield something similiar.