Always start at 0-0-0?? Love Spoon Project

This section is for useful tips and tricks for Aspire
Post Reply
wood_fly
Posts: 8
Joined: Tue Jan 24, 2012 8:42 am
Model of CNC Machine: Shark Pro Plus HD

Always start at 0-0-0?? Love Spoon Project

Post by wood_fly »

Greetings,
I am machining a two-sided 1" thick project. For the front side, I am indexing in the middle of the project on the TOP of the project. I cut the dowel holes, and remove the material.
I put a sacrificial board on the bed and clamp it down. I then register 0-0-0 x-y-z on the middle of the sacrificial board and cut the matching, mirrored dowel holes.

Then I install my project board upside-down. I am still using the sacrificial board as my Z-0, and telling Aspire to set the home-start position at 0-0-1.2.

When the project starts however, the bit runs right to 0-0-0 and IGNORES the command to home of 0-0-1.2. The front of the G-code looks like this:
( 2 Back-Ruf-Z )
( File created: Sunday, December 15, 2013 - 11:08 AM)
( for CNC Shark from Vectric )
( Material Size)
( X= 6.000, Y= 21.000, Z= 1.000)
( Z Origin for Material = Table Surface)
( XY Origin for Material = Center)
( XY Origin Position = X:0.000, Y:0.000)
( Home Position)
( X = X0.0000 Y = Y0.0000 Z = Z1.2010)
( Safe Z = 1.200)
(. IMPORTANT: Before outputting any toolpaths you)
(should carefully check all sizes and the material)
(setup to make sure they are appropraite for your)
(actual material and CNC. You should also check and)
(re-calculate all toolpaths with safe and approprate )
(settings for your material, machine and tooling.)
(Terms of Use: This Project and artwork is provided )
(on the understanding that it will only be used with )
(Vectric software programs. You may use the )
(designs to carve parts for sale but the Files )
(and/or Vectors, Components or Toolpaths)
(within them {or any derivatives} may not be sold )
(to, or shared with anyone else. This project is )
(Copyright 2013 - Vectric Ltd.)
(Toolpaths used in this file:)
(2 Back-Ruf-Z)
(Tools used in this file: )
(1 = End Mill {0.25 inch})
(End Mill {0.25 inch})
(|---------------------------------------)
(| Toolpath:- '2 Back-Ruf-Z' )
(|---------------------------------------)
G90
G20
F100.0
G64 P.01
S 2000
M3
G0 Z1.2010

Does the CNC shark control panel ALWAYS issue a GOTO 0-0-0? I tried to slow down the software (25%) was the lowest and it looks like it stops on line 2 while sending the bit into the material seeking 0-0-0. I have ruined this project and won't try again until I can figure this out. HELP!

Thanks

User avatar
zeeway
Vectric Wizard
Posts: 3157
Joined: Thu Feb 11, 2010 9:24 pm
Model of CNC Machine: Self-built
Location: SC, USA

Re: Always start at 0-0-0?? Love Spoon Project

Post by zeeway »

Your g-code comments say that z zero is referencing to the table surface, but you say you are referencing z zero to the top of the material. Those two need to be the same. Home position is not the "origin".

Angie

wood_fly
Posts: 8
Joined: Tue Jan 24, 2012 8:42 am
Model of CNC Machine: Shark Pro Plus HD

Re: Always start at 0-0-0?? Love Spoon Project

Post by wood_fly »

From what I read, if you are machining a 2 sided surface, you define the "top" as the Z0 position. When you flip it over, the top is now on your table, so the table needs to be the Z0 position. That way, you are referencing the same plane when cutting the back as the front and minor differences in material thickness become irrelevant.

I (think) I understand "origin" as being the design "zero" in terms of how the project is designed. BUT I was under the impression that you could use the "home" position above the project. In my case, the CNC machine is going to 0-0-0 before it even reads the file (or so it would appear)

Perhaps my only option is to always reference off the top of the project. The board will have to be EXACTLY the proper dimensions or when it flips there will be a "mold line" where the two halves meet.

User avatar
zeeway
Vectric Wizard
Posts: 3157
Joined: Thu Feb 11, 2010 9:24 pm
Model of CNC Machine: Self-built
Location: SC, USA

Re: Always start at 0-0-0?? Love Spoon Project

Post by zeeway »

If you are machining a two sided project, I would first define in the job setup description that z zero is on the top of the material. Then I would physically zero z to the top of the material, and machine side 1.

Then I would flip it over and redefine the jb setup description to define z zero as the top of the table. Then I would recalculate the toolpaths so that they would be consistent with the new z zero position. Then I would physically zero z to the top of the table, and machine side 2.

If needed, the software will automatically adjust the home position so that it will clear the material - it will ask you if that is okay..and you would say 'yes'.

This all presumes that you have locating dowel holes from side one that you use to maintain registration when you flip the project to side two.

Angie

ps - it sounds like you are changing the home position, and thinking that this will change the origin position...it will not.

wood_fly
Posts: 8
Joined: Tue Jan 24, 2012 8:42 am
Model of CNC Machine: Shark Pro Plus HD

Re: Always start at 0-0-0?? Love Spoon Project

Post by wood_fly »

"If you are machining a two sided project, I would first define in the job setup description that z zero is on the top of the material. Then I would physically zero z to the top of the material, and machine side 1.

Then I would flip it over and redefine the jb setup description to define z zero as the top of the table. Then I would recalculate the toolpaths so that they would be consistent with the new z zero position. Then I would physically zero z to the top of the table, and machine side 2.

I believe I did exactly as you proposed and that is how the original Love spoon files are setup.

Bottom line: the CNC shark software ALWAYS goes to 0-0-0 on start regardless of what is written in the TAP file. It goes to 0-0-0 (which is the table) even before advancing through the lines of code. So I'm stuck referencing the top of the material it appears. If you read the first few lines of code, NOTHING there appears to send my CNC to 0-0-0 yet it does.

wood_fly
Posts: 8
Joined: Tue Jan 24, 2012 8:42 am
Model of CNC Machine: Shark Pro Plus HD

Re: Always start at 0-0-0?? Love Spoon Project

Post by wood_fly »

I was able to get some insight. The Shark CNC controller ALWAYS goes to 0-0-0 to start - regardless of what the rest of the software tells it to do. So I was telling it to do the right thing and it was saying, "Just a minute, I have to do this first because it's hard coded into my brain, then I'll follow your instructions." Almost as good a computer...oh wait...

The workaround is to use the "offset" feature in the setup panel and put the start position OFF the work and on the table surface. Then it can go there to start and lift up before moving over the project. At lest that's the theory. I'll let you know how it goes.

User avatar
zeeway
Vectric Wizard
Posts: 3157
Joined: Thu Feb 11, 2010 9:24 pm
Model of CNC Machine: Self-built
Location: SC, USA

Re: Always start at 0-0-0?? Love Spoon Project

Post by zeeway »

Bitten by the shark... :) ...glad to hear you are figuring out those shark-specific things. Presume you are also asking these questions on the shark forum.

Angie

User avatar
Norb
Vectric Craftsman
Posts: 202
Joined: Wed Aug 05, 2009 8:07 pm
Model of CNC Machine: MAXI-C 1530 SE-T-V
Location: Barbados

Re: Always start at 0-0-0?? Love Spoon Project

Post by Norb »

A few years ago I did a 44'' airplane prop. For both front and back I set the Z zero to the top of the material.

I entered the actual material thickness then.......

For side A, I ticked "Gap above Model" in "Model position in material" (Material Setup) and entered 0 (now take a note of the distance indicated in greyed-out field of "Gap below model")
and for side B, I used, of course, the same material thickness then in "Gap above Model" I entered the distance previously noted.

I still have prototype in my office. Looks great.
Norbert
Aspire 4.x, PartMasterCAM Turn, Autocabinets
after hours: Sherline 2010 and 4410

User avatar
Ms Wolffie
Vectric Wizard
Posts: 2689
Joined: Sat Mar 31, 2012 10:41 pm
Model of CNC Machine: Blue Elephant 1325, Shark HD Pro
Location: Tully Heads, Wet Tropics, Queensland, Australia

Re: Always start at 0-0-0?? Love Spoon Project

Post by Ms Wolffie »

wood_fly wrote:I was able to get some insight. The Shark CNC controller ALWAYS goes to 0-0-0 to start - regardless of what the rest of the software tells it to do. So I was telling it to do the right thing and it was saying, "Just a minute, I have to do this first because it's hard coded into my brain, then I'll follow your instructions." Almost as good a computer...oh wait...

The workaround is to use the "offset" feature in the setup panel and put the start position OFF the work and on the table surface. Then it can go there to start and lift up before moving over the project. At lest that's the theory. I'll let you know how it goes.
Correction
The Shark CNC Controller always goes to 000 to start. Not quite right.
The Shark always go to 000 wherever you have set it in your Material setup.
If you set 000 to the top of the material for your top model and save the toolpaths, then you can change the 000 to the table top for the second part, calculate the toolpaths and save them.
After you change the 000 the program will tell you to reset all toolpaths, just ignore that as you have already saved the first toolpaths.
Cheers
Wolffie
Cheers
Wolffie

Whatshammacallit
Cut3D, VCarvePro 6.5, Aspire4, PhotoVCarve, Corel Graphics Suite X6

wood_fly
Posts: 8
Joined: Tue Jan 24, 2012 8:42 am
Model of CNC Machine: Shark Pro Plus HD

Re: Always start at 0-0-0?? Love Spoon Project

Post by wood_fly »

To be clear, using the shark controller software, wherever you set 000 is where the tool will go when you run a toolpath REGARDLESS of what your g-code file is set. I confirmed that with the manufacturer.

In Aspire, I set the material setup to reference the middle of the project and the Z-top of the board. Then I saved the toolpaths, set 000 in the machine controller and ran the top side.
Then in Aspire, I set the material setup to the Z-bottom of the board, face now on the table, to reference the same face. I also set the "Safe/home" position to 0-0-1.2 (1" thick board) in Aspire. I set the controller software to reference 000 on the table and ran the project. I set the controller to it's slowest setting to I could watch how it executed the instructions.

While the window showed line 1 of the code was active (which is in the comments section), the bit ran right through the project seeking the table. THEN it ran down to line 40 in the code and went to 0-0-1.2 and remained nice and high for the remainder of the cutting. Now I have a very nice 3D spoon with a convenient hole in the middle for mounting.

wood_fly
Posts: 8
Joined: Tue Jan 24, 2012 8:42 am
Model of CNC Machine: Shark Pro Plus HD

Re: Always start at 0-0-0?? Love Spoon Project

Post by wood_fly »

Norb wrote:A few years ago I did a 44'' airplane prop. For both front and back I set the Z zero to the top of the material.

I entered the actual material thickness then.......

For side A, I ticked "Gap above Model" in "Model position in material" (Material Setup) and entered 0 (now take a note of the distance indicated in greyed-out field of "Gap below model")
and for side B, I used, of course, the same material thickness then in "Gap above Model" I entered the distance previously noted.

I still have prototype in my office. Looks great.
That's awesome - simple and elegant. I LIKE IT. Thank you (and a prop at that. This aviator thanks you and wants to make one of his own...hmmm :idea: )
Tim

Post Reply