Profile cut - Last pass seems to speed up.

This forum is for general discussion regarding VCarve Pro
flying_flip
Vectric Apprentice
Posts: 58
Joined: Wed Feb 15, 2017 10:38 pm
Model of CNC Machine: Piranha FX / VCarve Desktop
Location: Tucson, Arizona

Profile cut - Last pass seems to speed up.

Post by flying_flip »

I have posted the the Vectric suport group this question, but thought I would post here as well.

I am using V-Carve Desktop version 9, and exporting my Project tool paths for a Piranha FX (in inches).
I have noticed that when cutting out the parts, that the last pass speeds up on my machine.
Not the router, but the motion of the machine.

Is this a problem with the G-Code generated, the machine, or …?

If I cut 2 circles, after completing the cut on the first circle, the machine seems to slow down to begin the cut of the second circle, but that last pass it speeds up.
I am not sure if this also occurs on Pockets. ( I hope to have a chance to get back in the shop this weekend.)

I would attach the G-Code generated, but do not have this file at work.
I hope to remember to bring the G-Code in tomorrow (and will post it for review).

Thanks,

Phil

User avatar
dwilli9013
Vectric Wizard
Posts: 1237
Joined: Mon Sep 30, 2013 12:45 am
Model of CNC Machine: 3 axis Self Designed Self Built
Location: Machesney Park Illinois

Re: Profile cut - Last pass seems to speed up.

Post by dwilli9013 »

Sounds to me as though you have ramps or lead ins set. This would exhibit the behavior you are seeing. :lol: :lol:
D-Dub
Dwayne
Dwilli

flying_flip
Vectric Apprentice
Posts: 58
Joined: Wed Feb 15, 2017 10:38 pm
Model of CNC Machine: Piranha FX / VCarve Desktop
Location: Tucson, Arizona

Re: Profile cut - Last pass seems to speed up.

Post by flying_flip »

I believe that ramping is set to spiral.
Is that what you mean?

User avatar
dwilli9013
Vectric Wizard
Posts: 1237
Joined: Mon Sep 30, 2013 12:45 am
Model of CNC Machine: 3 axis Self Designed Self Built
Location: Machesney Park Illinois

Re: Profile cut - Last pass seems to speed up.

Post by dwilli9013 »

Yes it can be spiral or linear. there is a setting where you can control the length of the ramp or lead in. The software then eases into the material at a slower feedrate in order to stop the bit from being side loaded all at once. Once it is to full DOC then it will continue on at the set feedrate. If you uncheck that I believe you would see it does indeed cut at the same speed throughout. Just be careful as eliminating the leads and ramps your bit will plunge to full depth and take off at full speed.
D-Dub
Dwayne
Dwilli

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: Profile cut - Last pass seems to speed up.

Post by Leo »

Not absolutely positive, but, I think if you increase your plunge feedrate to be at least close to the XY feedrate the result would be a more uniform feedrate all the way through the spiral. I am pretty sure the plunge feedrate in influencing the spiral overall. When you are no longer plunging the XY feed rate is no longer influenced and it picks up the full speed.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: Profile cut - Last pass seems to speed up.

Post by ger21 »

A spiral lead in will be made up of short, straight G1 moves, and your control may not run as fast through those as the final G2/G3's for the circle.
Gerry - http://www.thecncwoodworker.com

flying_flip
Vectric Apprentice
Posts: 58
Joined: Wed Feb 15, 2017 10:38 pm
Model of CNC Machine: Piranha FX / VCarve Desktop
Location: Tucson, Arizona

Re: Profile cut - Last pass seems to speed up.

Post by flying_flip »

Going by memory right now,
but I think back when I setup my tool database that I set the plunge to half the feed rate for all bits, so that makes sense now...

It does make sense that the spiral is (should be) influenced by the plunge.

Okay then.
I will review my setup in the software tonight, and report back.
With Spiral, I'm thinking that ramp distance and angle get grayed out.

Thanks everyone.

Phil

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: Profile cut - Last pass seems to speed up.

Post by Leo »

OK - I was wrong.

Ger21 is correct - but

I just created a toolpath to spiral down a circle

The tool moves in RAPID to XY = 0 - center of my circle, because I set center as zero. Then the tool moves in RAPID to a position to start cutting. At that point it goes into the spiral cutting at the programmed PLUNGE feedrate just as GER21 said - G1 straight XYZ moves AT THE PLUNGE feed rate.

That's OK. Most of these machines do not have "helical" cutting capabilities, so a G3 with "Z" really cannot be done.

At the bottom the XY feedrate then takes over and there is a few G3 XY circular moves AT THE XY FEEDRATE.

So - the spiral feedrate is not influenced by the plunge rate - it in fact IS the plunge feedrate.

Be careful with increasing the plunge feed as the cutters do not have the gullet clearance to evacuate chips in a plunge cut as they do with perifery cutting. Spiraling is a little different, but it is still plunging.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Profile cut - Last pass seems to speed up.

Post by IslaWW »

To add to Ger's info, there are 3 different scenarios that occur when cutting a spiral segmented circle with a G2/3 final pass. I'm leaving the lack of G2/3 with Z depth for another day.

First scenario: As Leo describes with the segmented (Z involved) portion of the cut being done at Z feedrate, G2/3 at bottom (no Z involvement) done at XY feedrate.

Second scenario: Segmented section is done at a reduced feedrate due to Z involvement, G2/3 at full feedrate

Third scenario: Segmented section done at feedrate, G2/3 section done at feedrate. Assumes that executing the spiral down segmented section does not cause Z to exceed its set feedrate.

What determines which scenario happens on your machine? The controller that you are using. They do not all react the same. Nor will they all react the same to a similar file that was posted with G2/3 arcs with z involvement.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

flying_flip
Vectric Apprentice
Posts: 58
Joined: Wed Feb 15, 2017 10:38 pm
Model of CNC Machine: Piranha FX / VCarve Desktop
Location: Tucson, Arizona

Re: Profile cut - Last pass seems to speed up.

Post by flying_flip »

Below is a portion of the tap file, where the F25 is still moving down, then transitioning to F75 on the final circle (with tabs).
One interesting note is that the Tool definition is 50/25 for Feed and plunge...

F25.0
G1 X0.6676 Y1.7186 Z-0.9936
F25.0
G1 X0.6752 Y1.6963 Z-0.9938
F25.0
G1 X0.6832 Y1.6741 Z-0.9941
F25.0
G1 X0.6914 Y1.6521 Z-0.9944
F25.0
G1 X0.7574 Y1.5012 Z-0.8668
F25.0
G1 X0.7973 Y1.4291 Z-0.8000
F25.0
G1 X0.8373 Y1.3569 Z-0.8668
F25.0
G1 X0.9303 Y1.2211 Z-1.0000
F75.0
G03 X2.3263 Y0.5265 I1.3959 J1.0554
G03 X3.7086 Y1.2033 I0.0000 J1.7500
F75.0
G01 X3.8034 Y1.3380 Z-0.8668
G01 X3.8443 Y1.4097 Z-0.8000
G01 X3.8852 Y1.4814 Z-0.8668
G01 X3.9531 Y1.6315 Z-1.0000
F75.0
G03 X4.0763 Y2.2765 I-1.6268 J0.6450
G03 X2.5566 Y4.0113 I-1.7500 J0.0000
F75.0
G01 X2.4417 Y4.0227 Z-0.9000
G01 X2.3263 Y4.0265 Z-0.8000
G01 X2.2109 Y4.0227 Z-0.9000
G01 X2.0960 Y4.0113 Z-1.0000
F75.0
G03 X0.5763 Y2.2765 I0.2303 J-1.7348
G03 X0.6914 Y1.6521 I1.7500 J0.0000
F75.0
G01 X0.7574 Y1.5012 Z-0.8668
G01 X0.7973 Y1.4291 Z-0.8000
G01 X0.8373 Y1.3569 Z-0.8668
G01 X0.9303 Y1.2211 Z-1.0000
F75.0
G00 X0.9303 Y1.2211 Z0.2000
G00 Z0.2000
G00 X0.0000 Y0.0000
M02

Thanks,

Phil

flying_flip
Vectric Apprentice
Posts: 58
Joined: Wed Feb 15, 2017 10:38 pm
Model of CNC Machine: Piranha FX / VCarve Desktop
Location: Tucson, Arizona

Re: Profile cut - Last pass seems to speed up.

Post by flying_flip »

flying_flip wrote:One interesting note is that the Tool definition is 50/25 for Feed and plunge...
I may be wrong here...

It is sure behaving like Leo notes.

Thanks again all, I have been playing with CNC since May, so still "learn'n the ropes"

Phil

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: Profile cut - Last pass seems to speed up.

Post by sharkcutup »

Just a comment here on the Spiral Ramp type

On the spiral type ramp profile cut I have always noticed that it ramps at Tool 'plunge feed rate' to the determined Tool 'cutting parameter pass depth' and continues at that cutting depth throughout the spiral plunge until it reaches the maximum cutting depth. Then once determined Tool 'cutting parameter pass depth' has been reached it no longer is plunging and picks up to Tool 'feed rate' completing the profile cut.

Since I have come across this type of profile cut I have continued to use it for most of my profile cutting for it seems to be the most efficient, (not the fastest by no means), but the most efficient profile cut. It is an efficient gradual type of cutting thereby minimizing edge chatter providing a clean edge.

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

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: Profile cut - Last pass seems to speed up.

Post by ger21 »

Leo wrote:
The tool moves in RAPID to XY = 0 - center of my circle, because I set center as zero. Then the tool moves in RAPID to a position to start cutting. At that point it goes into the spiral cutting at the programmed PLUNGE feedrate just as GER21 said - G1 straight XYZ moves AT THE PLUNGE feed rate.

That's OK. Most of these machines do not have "helical" cutting capabilities, so a G3 with "Z" really cannot be done.
Actually Leo, I think that most hobby controls DO support helical G2/G3 moves, and it would be nice if Vectric gave that as an option.
Gerry - http://www.thecncwoodworker.com

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Profile cut - Last pass seems to speed up.

Post by IslaWW »

I am not positive, but the ONLY one that I am aware that does NOT support helical G2/3 commands is ShopBot. There is a possibility that their new FabMo system will support this very common and sadly missing from Vectric's arsenal often used feature.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
Adrian
Vectric Archimage
Posts: 14541
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Profile cut - Last pass seems to speed up.

Post by Adrian »

I haven't used it personally as it's not supported by Vectric but the ShopBot G2/G3 equivalent has plunge (z) parameters available. I always thought that specifying a Z on a G2 or G3 (or with the SB CC/CG commands) would plunge to that depth and cut the arc rather than "spread" the plunge over the arc length. I should give it a go really as it would be useful for a few of the carbon fibre jobs I do.

Post Reply