Help needed With 120 Deg V- Bit

[Captive]

So I am trying to essential cut some prism type shapes with a 120 deg V-Bit. I am cutting out the shape using a profile and flute tool path in V carve pro. However when I cut the flute tool path to create the sharp internal corners for whatever reason it creates a little dimple at the peak where the two prisms should meet….. I am at a loss why this is happening.

Here is what I have done.
Double check thickness of Zero plate.
Zero the bit to top of material with out using zero plate.
Adjust the angle of the bit + or – a few degrees but it did not make things better.
Also adjust the feeds and speeds with regards to flute tool path but again no real benefit.

I have tried to cut this several times and each time I get a bit of a different result but every time there are some type of dimples where there is the flute tool path… this is leading me to think that it’s a material or tool issue but I can’t seem to figure it out…. I attached some photos hope this helps…

Any advice would be appreciated….

[rcnewcomb]

I have tried to cut this several times and each time I get a bit of a different result
My guess is your material is moving a little bit. What is your hold down method? Clamps? Screws? Vacuum? Double-sided tape?

[steve_g]

Another possibility…
Judging by the “water marks”, there’s the possibility that your bit isn’t a true 120°. Try redefining the bit as 121° and see if it’s better or worse… if worse try 119°, and so on…
SG

[Captive]

I have been using clamps to hold down the material but perhaps I will try this again and add a few more.

I tried changing the the angle of the bit but no luck still got the same results... I even tried this this with a different 120 V bits and I keep getting these dimples....

[coryatjohn]

Do you see it in preview as well? Do you see the bit doing something odd in that spot or is the material popping off?

[paul_z]

Using sharp corners on vectors which do not form a closed polygon can cause exactly this problem. I reported it as a bug but I don't think they intend to fix it. Instead, they'll pop up a warning message.

You may be able to get what you want by computing two offset vectors and profile cut those "on the line". If you need help with the math, just let me know.

Paul Z

[jerry_stanek]

I would move the bit to a spot that you know the location on your table and drill a small hole. After you run the file let the router go back home then move it to that spot to see if you had lost any steps

[Captive]

Coryatjohn,
I attached a 2 pictures of the preview… I check this and it does not do anything odd, in fact the edges look clean and crisp.

Pau_Z
I drew this using straight line vectors and the flute tool path… I tried to use the “ sharp corners” but it would not work for me with the open vectors… I attached a picture of the drawing.

Jerry_stanek
I will give this a shot see if I am losing any steps… the machine is PRS Alpha and I am cutting this a 3 ips…so I don’t think that would be aggressive enough to loss steps.. but I will give your idea a try…

270372703827039

[bleeth]

As this is mdf you very likely could be dealing with your part cupping a bit from stress relief as you remove material.
You might try screwing it down across / above your final cutout.
Also, since this is mdf, some careful hand work and/or bondo could fix it in a couple minutes.

[coryatjohn]

I'd go with Bleeth's suggestion. I doubt it would take much effort to hand carve the tips of your project with a file or xacto knife.

[Rob Gunn]

Captive, I may be wrong but it looks like bit deflection to me. No matter how rigid a machine is, you will always have a certain amount of side pressure on a tool while its cutting. This is what I would try, Run your tool path the same as what you have already done but have the Z-0 set about .05 high. Basically this is going to be your "roughing out cut". Then re-zero your Z down to your actual desired hight and re-run your same tool path. This is now just taking a small .050 light cut with much less tool side pressure. Some times I even run a 3rd final pass to remove just a very light cut of .010 but not always needed. I all depends on the cutter, the hardness of the material I am cutting, and how sharp and crisp I want to see the edges. Just my 2 cents worth. Let us know how it turns out.

[Brady Watson]

I didn't see any mention of cut speed. V-carving is best done at a low move speed (like MS, 1, 0.5) and 15k+ RPM depending on the material. There really isn't any cutting being done at the tip since there is no cutting flute; instead, it scrapes the surface. If your bit is dull, RPM too low and/or move speed too fast, it can cause the symptoms you show, like knocking off the apex etc.

Try just a small portion at a lower speed with higher RPM & see if it helps.

-B

[Captive]

Just want to say thanks for everyone for there help with this….I got a chance to work on this again today and still getting the same results….here is what I did.

1) Used a few more clamps to hold down my material to make sure it did not move.
2) Change the program so that the flute tool path is being cut last so that the flute tool path removes less material hence reducing the chance of deflection.
3) Changed the feed / speed to 1 ips at 15000 rpm… the flute I cut at 0.5 ips…as per what your recommended, Brady…..if I understood it correctly
4) Make a last pass to remove 0.05 worth of material to again reduce bit deflection.

I also did a few cuts to double check the geometry of the bit by cutting to a depth of 0.25 then using some Trigonometry to calculate what the width of the groove should be and check it with my calipers and it was correct… so according to my math the bit I am using is 120 degrees
The only deference I noticed is this time the dimples are a consistent is size and happened every time as before they were bigger and smaller so to speak…. I cut this out about 4 times today, each time changing something and on the last cut implementing all the points… I attached a few pictures of the last part I cut…… if any one has any other ideas I be more than happy to hear them… thanks
270512705227053

[RossMosh]

Have you tried just doing a profile pass and use a little geometry to figure the offset?

[Captive]

RossMosh

I am not sure I know what you mean...can you explain a bit more...thanks

[RossMosh]

Can you post a vector file and let me know what pocket depth you're doing? I'll give my idea a shot and show you what I mean.

[Captive]

I should also add I learned another very import lesson... double check your numbers when changing VA values.... attached is a pic... I meant to change Z to 1.05 but i think i changed it to 10.5.... yeah.. it was not good...27054

[scottp55]

Make sure you clean/inspect collet/spindle nut/spindle cone after a burn like that.
You'd be amazed at the gunk on the paper towel/Q-tip from the smoke.
Did the same move on mine(but a little worse on Teak 1.0" instead of .1" cut) and had to chuck my nut and collet as I couldn't even get them apart until I soaked them.
Funny how you remember these lessons about pesky little Z decimal points:)
Cut it out and put on your wall for a reminder.
scott

[Brady Watson]

What does the simulation look like in VCP? Does it show the divots? It's nearly 100% spot on in terms of what you see is what you get at the machine. I'm sure you looked at this, but it doesn't hurt to check again zoomed in at each problem location.

The other thing could be that the vectors themselves are causing issues, although this *should* show up in the preview.

Have you given your machine a good 'shake down' to make sure that nothing is loose with the motors powered on & not moving?

-B

[Captive]

Brady,

I have look at the simulation a few times and it does not show the divots... and I just checked this again and no divots..

I think I might try re-draw this from the start just in case I did something funny with the vectors that I am not catching....

As for a " shake down" on the machine is there anything you could recommend to check. The Machine is a PRS alpha 48x96 only a few months old and I would even say less then 200 hours of use on.... it all seems pretty solid to me but I would appreciate any suggestions.....

[Burkhardt]

Is the divot machined in the course of the normal contiguous v-carve process or does it maybe happen while the bit traverses from the end of one segment to the beginning of the next? I know, wild guess...

[scottp55]

Make sure you are running latest version VCP8. There was a glitch right up through Vers. 8.016 that Z didn't retract completely when VCarving in a pocket.
Latest is VCP8.024.
8.024 and the glitch never showed again. Probably not it as preview DID show it, But...
What G. said reminded me of it.
scott

[Joe Porter]

You mentioned you were using a profile and fluting toolpaths. Can you do this with the V-Carve method of toolpathing and get better results? I think people use fluting toolpaths to simulate 3D cutting in V-Carve...just a thought...joe

[Captive]

Burkhardt,
Iam cutting this with a profile & fluting tool path and it happens during the fluting tool path, thats when it happens...am I understanding what you are asking correctly ?

Scottp55,
Just checked and have the most current VCP8 024 version on my system.

Joe,
I will try to see if I can do this with a V-Carve tool path and see what I get

Thanks again for everyones idea

[Captive]

So I made some more test cuts today with a 120 Deg bit and 90 Deg bit using sharp internal corners and cut just a basic letter “ C” shape and I attached in the pictures are the results…. Its obviously way off from what should be sharp corners. These is leading me to think the problem is not a tool or software problem but rather a mechanical problem. ( RPR 15000, 1 ips )

Does anyone have any ideas on what to start Checking first ?…. Thanks


27109
2711027111

[Brady Watson]

What machine do you have? PRT or PRS Gantry tool, PRT Benchtop, PRS Buddy, Desktop ???

If it is a PRS first guess is the lower V-roller bearings are loose. If PRT, T-rail is worn out letting it do the watoosie...

-B

[Burkhardt]

Now that is a puzzler....While I would not preclude a mechanical issue I wonder why that would show up only in right hand turn corners (assuming a counter-clockwise direction) and not on left hand turns. Also, the irregular machining spot is so symmetrical and well defined. If there was something loose in your machine I would suspect the trace to be wobbly or make an unsymmetrical excursion at the corner. That said, I still have no clue what can cause that.

What happens if you run the tool path with a small end mill?

Can you try a slo-mo video clip. Newer phones can do that.

[Captive]

The machine I have is a PRS Alpha... only a few months old, and less then 150 hours of cut time on it. I checked the V-rollers bearings on the Y-Car and they are tight... no play that I could feel. I even disconnected the Y motor and moved the Y car up and down along the Y axis to make sure it moved with out feeling loose or any binding... and if felt fine.

Brady,

Are you thinking the lower V-roller bearings on the Z-axis are loose ?.... I have not adjusted those yet

This cut was made in counter clock wise direction but I did not try any internal corner the other way ie a mirror of the picture so I don't yet know if it would do it in that direction as well.

As for cutting with a end mill.. everything else I have cut came out fine and I have not noticed and issues except for now when I have started to try use internal corners for a project....

[Captive]

Burkhardt

I re-read your post again.... I will try cut this out with and endmill tomarrow...and if I can post a video...if not photos..But when I was watching it closely it causes that odd divot in the material when and only when it is moving in the 3D motion to create the sharp corner...

[Captive]

Machine is a PRS Alpha Gantry 48x 96

[steve_g]

Captive…
Where are you z-zeroing your bit? Top of material?
SG

[Captive]

Yes, Top or the material

[scottp55]

Captive,
Wouldn't hurt to post that "C" file on the Vectric forum for people to look at.
Include the toolpaths.
VERY helpful guys, and a couple of Guru's.
scott

[Captive]

!!!!!!! SOLVED !!!!!!!

Well after a fair bit of trouble shooting and bit of frustration I believe I got it figured out.
I needed to adjust the " Z" axis Bearings as per the document on the shopbot web site.
I removed the Y motor, then loosened all the Z axis bearing then snugged them up and got the results I was looking for on the first shot.... which almost never happens .... attached are a few pictures...

So hopefully some one finds the thread of use in the future271212712227123

[Brady Watson]

Good!

It's a great time for EVERYONE to do some machine maintenance....

-B

[rgreever]

Glad you got it figured out, Captive! I've been following your progress, and vicariously feeling your pain and frustrations, lol.
I think my z-axis bearings might need some adjusting, as well. It looks like I have to remove the spindle to get to them. Is that the case?

[Brady Watson]

It looks like I have to remove the spindle to get to them. Is that the case?

No. On a PRS, they are underneath the beam. You have to take the Y-roller covers off if they came equipped. DON'T adjust them too tight!

On a PRT, you have to adjust the rollers very carefully on the Z. If you don't have 8 rollers, get them. They easily double the life of the T-rail. You need to adjust Y+ and Y- orineted rollers on the Z at the same time, clocking them in the exact same way. You also need to be mindful of the Z rack gear to Z pinion lash to make sure it isn't too loose or tight. You also need to make sure the Z rides true and perpendicular in XZ and YZ planes (square to table). You don't want these rollers too tight either because you can wear out the t-rail by roll forging...8 rollers helps. It is only necessary to remove the t-rail during this process (drop it out the bottom) in order to adjust the Z motor for gear lash.

-B

[Captive]

regreever

I did not take the spindle off... . There is a document on the shopbot web site...http://www.shopbottools.com/ShopBotDocs/gantry.htm the document name is "adjusting Z car bearings". Just follow the document its pretty straight forward... but it is VERY !!! easy to over tighten the bearings so just be aware of that...

[rb99]

Could you tell it was loose by moving it?

[Captive]

No,... it felt fine.. I real can't say if before I adjusted the bearings they were to tight or loose, I just loossened them all and then snugged them back up...hope this helps