Strange Occurance

This forum is for general discussion regarding VCarve Pro
Post Reply
User avatar
BArnold
Vectric Craftsman
Posts: 189
Joined: Sat May 02, 2015 12:20 am
Model of CNC Machine: SO2/XCarve hybrid w/NEMA23 on all axes
Location: Thomasville, GA, USA

Strange Occurance

Post by BArnold »

I just had a strange thing happen on a cut. I'm trying to carve radius rails for two door panels. They are 3/4" thick by 1.5" wide by about 6.75" long. All looked fine on my drawing and preview in VC, but when I started the carve on my CNC, I got the results below. When the carve started, it was cutting only 5/8" wide for the first four passes. The remaining nine passes were cut at about 11/16". It should have cut at 3/4" thick all the way through.
Top of work piece
Top of work piece
Bottom of work piece
Bottom of work piece
Here are the settings I'm using.
Screenshot of VCarve settings
Screenshot of VCarve settings
What might I be missing?
Bill Arnold
VCarvePro, PhotoVCarve, SketchUp, UGS
Member of Mensa and NRA

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Strange Occurance

Post by Leo »

Bill,

I can think of several things.

Can you post the v-carve program .crv file?

First off the cuts look rough, maybe I am not seeing it well enough.

How are you holding it in the machine?

There may be some flexing of the material, or the machine.

Do you have a good sharp cutter?

Posting the .crv file will also help answer questions

How is you machine calibration? Have you checked to see if the machine accurately cuts a circle or a square?
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
BArnold
Vectric Craftsman
Posts: 189
Joined: Sat May 02, 2015 12:20 am
Model of CNC Machine: SO2/XCarve hybrid w/NEMA23 on all axes
Location: Thomasville, GA, USA

Re: Strange Occurance

Post by BArnold »

Leo, thanks for responding.

Everything else I've cut has been accurate in all ways. The length of this piece is perfect. I used the bit to cut other radius pieces for this project and had no problem.

The bit I'm using is good; it cut well when using it on my router table. I had the work piece (cherry) screwed directly to the MDF base board of my machine. I should have hit the piece with some 220 grit to clean it up a little.

I have other 1/4" bits. I'll run another test today with one of those to be sure about it.

My first thought was, "What did I get wrong in the .crv file?" If there's a problem with it, I haven't seen it yet.

Here's my .crv file:
DoorRails.crv
(595 KiB) Downloaded 115 times
Bill Arnold
VCarvePro, PhotoVCarve, SketchUp, UGS
Member of Mensa and NRA

User avatar
sharkcutup
Vectric Wizard
Posts: 2885
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Location: U.S.A.

Re: Strange Occurance

Post by sharkcutup »

After reviewing your .crv file

I am noticing that not only are you cutting a very thick material but you are also cutting along the grain structure of the material at a relatively high feed speed. Even with the sharpest cutters cutting along the grain there is some resistance due to grain structure. There is also no ramp into cutting the part just a plunge whereas on a plunge with the combination of machine flex the start of a cut can vary. Also one other thing I do not see here is the actual bit size. There is .1463 - .1445 difference in the drawing width size and actual material cutting size. Make sure you are using/and inputting correct bit size.

Granted ramping versus plunge into a part takes time but it can help with providing an accurate cutting position start. But if your bit is not measured to the correct size that could also affect the cutting dimensions.

Also what is the cutting length of the bit being used?? The longer the bit the more susceptible the carving results are to machine flexing.

These are just a few of my opinions/thoughts!

Have a Great Day!

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

User avatar
SteveNelson46
Vectric Wizard
Posts: 2282
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger 1
Location: Tucson, Az.

Re: Strange Occurance

Post by SteveNelson46 »

That's a hell of a warp in that board! Obviously, the depth of the cut will depend on where you set your z-zero. The warp may not be symmetrical so when you flip the board over...
Last edited by SteveNelson46 on Sat Aug 11, 2018 4:31 pm, edited 1 time in total.
Steve

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Strange Occurance

Post by Leo »

Bill,

I don't see anything wrong in the CRV file. A bit fast on the feedrate maybe.

As the other poster mentioned about bit sizes, I don't see anything wrong there either. The actual bit would need to be about .06 larger diameter than .25 to cause the problem that you are seeing.

You are set to conventional cutting. Maybe Climb cutting will help. I am climb cutting almost exclusively.

You have said that the machine accuracy is good. I am assuming that you did some test cutting and actually measured to determine the accuracy.

Over all though, it sounds like the part is moving as it is being cut. It is a better dimension where the screws are holding, and does it taper smaller at the top of the cut?
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
BArnold
Vectric Craftsman
Posts: 189
Joined: Sat May 02, 2015 12:20 am
Model of CNC Machine: SO2/XCarve hybrid w/NEMA23 on all axes
Location: Thomasville, GA, USA

Re: Strange Occurance

Post by BArnold »

sharkcutup wrote:... I am noticing that not only are you cutting a very thick material but you are also cutting along the grain structure of the material at a relatively high feed speed. Even with the sharpest cutters cutting along the grain there is some resistance due to grain structure. There is also no ramp into cutting the part just a plunge whereas on a plunge with the combination of machine flex the start of a cut can vary. Also one other thing I do not see here is the actual bit size. There is .1463 - .1445 difference in the drawing width size and actual material cutting size. Make sure you are using/and inputting correct bit size. ...
The board I'm cutting is 1.5" thick. I've cut other radius pieces that were 1.25" thick with no problem. I adjusted the feed rate down to 60ipm, used ramps and got a better cut; still not perfect, but better. The bit I used measures 1/4" and the cut it makes measures 1/4" exactly. Changing to a climb cut as Leo suggested also seemed to help, but the part came out a little oversized. More testing to be done.

I know my CNC makes good circle and radius cuts. The items below were made on it and measured exactly what they were designed to be.
ShelfParts_a .jpg
Bill Arnold
VCarvePro, PhotoVCarve, SketchUp, UGS
Member of Mensa and NRA

User avatar
BArnold
Vectric Craftsman
Posts: 189
Joined: Sat May 02, 2015 12:20 am
Model of CNC Machine: SO2/XCarve hybrid w/NEMA23 on all axes
Location: Thomasville, GA, USA

Re: Strange Occurance

Post by BArnold »

SteveNelson46 wrote:That's a hell of a warp in that board! Obviously, the depth of the cut will depend on where you set your z-zero. The warp may not be symmetrical so when you flip the board over...
That "warp" is called a 40" radius arc. The piece is a rail for a cabinet door I designed.

The board is dead flat. I flattened a face on my joiner, then ran it through my planer to make the faces parallel.
Bill Arnold
VCarvePro, PhotoVCarve, SketchUp, UGS
Member of Mensa and NRA

ElevationCreations
Vectric Craftsman
Posts: 180
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Strange Occurance

Post by ElevationCreations »

.The board I'm cutting is 1.5" thick. I've cut other radius pieces that were 1.25" thick with no problem.
What length of cutter are you using and what is the flute length?

A work around may be to do a pocket cut oversized and then a final profile cut to minimize any binding and help with chip clearance.

You may also want to change your DOC to a little less and see if that helps as well.

User avatar
SteveNelson46
Vectric Wizard
Posts: 2282
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger 1
Location: Tucson, Az.

Re: Strange Occurance

Post by SteveNelson46 »

BArnold wrote:
SteveNelson46 wrote:That's a hell of a warp in that board! Obviously, the depth of the cut will depend on where you set your z-zero. The warp may not be symmetrical so when you flip the board over...
That "warp" is called a 40" radius arc. The piece is a rail for a cabinet door I designed.

The board is dead flat. I flattened a face on my joiner, then ran it through my planer to make the faces parallel.
Ah! Now I see.
Steve

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Strange Occurance

Post by FixitMike »

One comment on your toolpaths. I would cut the Dado first, before the pieces are profiled and held only by the tabs.
And as others have pointed out, the profile is an pretty deep cut for a 1/4" bit.
Good judgement comes from experience.
Experience comes from bad judgement.

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Strange Occurance

Post by FixitMike »

More:
You have Conventional selected for the cutting direction. The cutting forces will tend to force the end of the bit inward, reducing the size of the profile. Climb will force the bit outwards,so it would probably end up with an oversize profile.

A suggestion: Offset the profiles outward by .28". Chose the new profiles and then the original profiles, and cut a a pocket. Check the "Use Vector Selection Order" box. This will double the time for cutting, but the final cut will be quite light, which will greatly reduce tool and machine deflection.
Good judgement comes from experience.
Experience comes from bad judgement.

User avatar
sharkcutup
Vectric Wizard
Posts: 2885
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Location: U.S.A.

Re: Strange Occurance

Post by sharkcutup »

This may take more time but it could help the overall part too. Make it a two-sided operation on the profile cut cut half one side then half on the other. That will also alleviate tool/machine deflection on cutting through such thick material.

Just another thought/opinion!!!

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

User avatar
BArnold
Vectric Craftsman
Posts: 189
Joined: Sat May 02, 2015 12:20 am
Model of CNC Machine: SO2/XCarve hybrid w/NEMA23 on all axes
Location: Thomasville, GA, USA

Re: Strange Occurance

Post by BArnold »

UPDATE:

I ran some tests today to determine what caused my issue. Although I had run some larger curved parts at the 100ipm feed rate with no problem, I slowed the cut on this smaller piece to 30ipm. That made a difference in the accuracy, but I also spotted another factor.

When going to the Toolpaths window and clicking on Material Setup, the Zero Gap Above Material defaulted to 0.80". On all items I've done until this one, that didn't seem to matter. My normal process for setting Z0 is to use a 1/2" block of wood with a piece of copper inset to Auto Set Z0. Part of the command set I use sets the block point to 0.5", raises the bit by 0.25" and sets that as the Z level. Because of the thickness of this item, I had to change the 0.25" to 0.1" to keep the router from crashing in to the top of my Z axis assembly. So, the combination of the ZGAM defaulting to 0.80" and my change in the offset I used in the Auto Set routine made the bit plunge about 0.25" into the material on the first pass rather than 0.0625" per the bit setting. After getting that straightened out, I got a good cut.

But, I have a question for you about the ZGAM number. I changed it from 0.80" to 0.0" and clicked OK. When I checked at the bottom of the Toolpath window, it showed the Home Position as Z0.21". Why does the software make that change?
Bill Arnold
VCarvePro, PhotoVCarve, SketchUp, UGS
Member of Mensa and NRA

Post Reply