Roughing, Finishing

McOtis
Posts: 80
Joined: Sun Feb 09, 2014 12:21 am
Location: Maryland

Re: Roughing, Finishing

Post by McOtis » Wed Sep 02, 2015 9:14 pm

Don't be intimated by learning Fusion 360. Luckily there are hours of YouTube videos on how to use the CAD and CAM features.
Fusion 360 and Easel are great.
Fusion 360 has a CAM setting to know what material is already milled away, and will adjust future operations accordingly;
Example - cutting a square pocket. Rough with a 1/4" bit and finish with a 1/8" doing the corners only. No wasted time cutting air.
Open Source is great and all, but as far as MakerCAM goes, it is long outdated and not worth using most of the time.
Sometimes I think it sours a newbie's experience due to its quirks and frustrations. However the same can be said with almost any software!

sraney
Posts: 43
Joined: Thu Mar 13, 2014 9:57 pm

Re: Roughing, Finishing

Post by sraney » Fri Sep 04, 2015 6:07 am

I think this kinda falls under the Roughing and Finishing subject line here, feel free to move it admin.

I have a procedure question on after you have a set of Roughing and Finishing jobs that have been exported from Fussion360, Aspire, or Cambam. if I run two jobs, a roughing and a finishing, the finishing job starts in the +x and +y position past the start of the rough job. I'm not sure if It's a problem with the gcode, or the home-spun procedure I use to change the tool. If requested I can include a very basic set of jobs as an example.


Here is how I have been starting my jobs.
  • Home my ShapeOko, X,Y, and Z (max)
  • Lower my Z Axis down using jogs to drop the tip of the Endmill to 0.051mm over the work-surface using a finger gauge
  • Enter G92 Z0.051 to reset my Z Axis to 0.051mm.
  • Mill a quick peck at 0,0 to verify I'm at the corner
  • Run my Roughing Job.
How I change my Endmil.
  • Enter G0 Z28 to lift my Endmil top 28mm over the surface
  • Change the Endmill to the smaller bit (a 0.029in ball) Carefully.
  • Enter GX0Y0 to mover the X and Y axis to 0,0
  • Repeat the peck to Validate it is over 0,0.
  • Lower my Z Axis down using jogs to drop the tip of the Endmill to 0.051mm over the work-surface using a finger gauge
  • Enter G92 Z0.051 to reset my Z Axis to 0.051mm.
  • Run my Finishing job.
-- This is wehre any job I create start off about +20X and +20Y off.

Just a few notes:
- My work-surface lower left hand corner is at 0.0.
- I am in G21 mode.
- And all my Stepper-Motors are engaged through out the job. To move an axis, I have to jog the positions around via control's or command.

Is this correct? Or is there an obvious error I am inducing with my procedure?
-- sraney
---------------------------------------
  • break nothing but silence
  • take nothing but pictures
  • leave nothing but footprints

RobCee
Posts: 587
Joined: Wed Jan 08, 2014 11:33 am
Location: Birmingham, UK

Re: Roughing, Finishing

Post by RobCee » Fri Sep 04, 2015 8:47 am

@sraney - Make sure to accommodate (or remove) any M30 command at the end of your roughing job, as it resets a lot of things.

M30 command will perform the following actions:

1. Change from Auto mode to MDI mode (Manual Data Input).

2. Origin offsets are set to the default (like G54).

3. Selected plane is set to XY plane (like G17).

4. Distance mode is set to absolute mode (like G90).

5. Feed rate mode is set to units per minute (like G94).

6. Feed and speed overrides are set to ON (like M48).

7. Cutter compensation is turned off (like G40).

8. The spindle is stopped (like M5).

9. The current motion mode is set to feed (like G1).

10. Coolant is turned off (like M9).


I find that when I use work coordinates and tool offsets, this command catches me out more than it should! It may not be helping your setup.
ShapeOko2 #3400 - Chinese 800W AC Spindle - Stiffened X-Axis - TR10 Z-Axis - Inverted Z Motor - Hall Effect Limits - Drag Chains & Custom Brackets

sjj47
Posts: 57
Joined: Thu Jul 02, 2015 10:40 pm

Re: Roughing, Finishing

Post by sjj47 » Sun Sep 06, 2015 12:44 am

WillAdams wrote:With the free programs, one usually has to manually break up the operations into different files.

In MakerCAM, I do this by importing the project once, doing all the roughing passes w/ a suitable roughing clearance, export to a suitably named Gcode file and resave the SVG to that same name w/ the .svg extension.

Then I reload the file, do all the finishing passes and export and resave under a second new name.
Newbie question. When I physically change bits -- from a 1/4" roughing bit to a 1/8" finish bit, say - I'm necessarily removing the router from the aluminum mount. That most likely throws off the origin point, right? How do I get the new bit positioned back to the same origin point as used for the roughing cut?

Do I just jog over to that point by eye? Or can I trust the offsets have remained correct while I wrestled with removing and reinstalling the router?
--------------------------------
Shapeoko 3 # 0761 - DW611 - Limit switches - probe
Current tool chains: Inkscape > MakerCAM > UGS | bCNC & F-Engrave > UGS | bCNC

WillAdams
Posts: 8628
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Roughing, Finishing

Post by WillAdams » Sun Sep 06, 2015 12:48 am

That's why I installed Tim's nift home/limit switches
Shapeoko 3XL #0006 w/ Carbide Compact Router w/0.125″ and ¼″ Carbide 3D precision collets

Estlcam
Posts: 89
Joined: Tue Sep 10, 2013 3:13 pm
Location: Germany
Contact:

Re: Roughing, Finishing

Post by Estlcam » Sun Sep 06, 2015 7:26 am

Hi,
2wistd wrote:I've seen people cut a shape with a 1/4 larger endmill, then cut the inside with a finer detailed endmill. I would like to cut a design into a thicker piece of wood and my endmills with smaller tips taper which doesn't allow me to use the same endmill to cut out the circle. How is this done?
you can do this with most CAM programs like e.g.Estlcam:
  • First you define your 2 (or more) tools in the tool list...
  • Then you just create your toolpaths and select the correct tool for each...
  • Tool changing code will automatically be inserted into the CNC program - so whenever a tool change is required the machine will stop and wait for you to change the tool.
  • All you need to do after changing is to zero the Z-axis again because the length the new tool sticks out of the collet will most likely be different to the last one. X and Y stay the same.
Here is a short Video showing the workflow in Estlcam: https://youtu.be/l48CfiVdzyg?t=38s

2wistd wrote: 2nd, Roughing, then finishing? I have only used SVG paths to Easel so far. I don't think it has the option to do so, what program does? Again how do I do this?
Programs with "automatic" roughing and finishing support are usually quite expensive - but if you don't mind to create the 2 steps separately it is also possible with Estlcam:
  • First you create a toolpath and set the desired "allowance" to leave some material like shown here: https://youtu.be/7_MlTtGU8_s?t=2m24s
    This will be the roughing toolpath...
  • Then you create a second toolpath (with the same or a different tool) without allowance which will be the finishing pass...
  • Finally you'll need to set the machining order properly so the roughing pass will be machined before the finishing pass...
I hope this wasn't too much of a commercial ;)
If there are any questions or problems just ask. You can also post a sample file and I'll try to show the workflow in a short video.
xfredericox wrote: But to answer your second question, there are no really useful free CAM pachages for 3D milling that I know of. I use RhinoCAM but that is rather expensive.
Not free but $50 and quite efficient: https://www.youtube.com/watch?v=xw0ZFf75lAM

Christian
Estlcam CAM and Arduino UNO CNC controller: www.estlcam.com

cvoinescu
Posts: 4442
Joined: Thu Jul 19, 2012 6:50 pm
Location: Camberley, UK
Contact:

Re: Roughing, Finishing

Post by cvoinescu » Mon Sep 07, 2015 9:12 am

sjj47 wrote:When I physically change bits -- from a 1/4" roughing bit to a 1/8" finish bit, say - I'm necessarily removing the router from the aluminum mount.
Why do you do that? Most people change bits without removing the router from the machine.
Proud owner of ShapeOko #709, eShapeOko #0, and of store.amberspyglass.co.uk

Georgei
Posts: 148
Joined: Mon Dec 22, 2014 11:22 pm
Location: UK

Re: Roughing, Finishing

Post by Georgei » Mon Sep 07, 2015 9:50 am

If you remove the router for every tool change you have a lot of work in your hands. You have to realign the router every time.

Nobody does that. I do not understand why you have to remove it.

Estlcam
Posts: 89
Joined: Tue Sep 10, 2013 3:13 pm
Location: Germany
Contact:

Re: Roughing, Finishing

Post by Estlcam » Tue Sep 08, 2015 7:12 am

Hi,
sjj47 wrote:When I physically change bits -- from a 1/4" roughing bit to a 1/8" finish bit, say - I'm necessarily removing the router from the aluminum mount. That most likely throws off the origin point, right? How do I get the new bit positioned back to the same origin point as used for the roughing cut?
you just move the Z-axis up and replace the tool with the router still in place. You can even move X and Y to a more convenient location.
After changing you just need to zero the Z-Axis again - because the new tool will most likely stick out of the collet at a different length than the last one.
You don't need to worry about X and Y - your CNC control software will remember the location before the tool change and automatically return to it.

Christian
Estlcam CAM and Arduino UNO CNC controller: www.estlcam.com

xfredericox
Posts: 292
Joined: Mon May 04, 2015 10:46 am

Re: Roughing, Finishing

Post by xfredericox » Tue Sep 08, 2015 12:40 pm

when I change bits, the carriage ends up displaced in the X-Y plane due to theforce applied to loosen the collet.

Makes re-aligning a real pain. My grbl-shield currents are at around 2-3 o'clock.

any ideas
Visit my blog for updates on my current SO2/lasercutting/... projects.
http://www.manmademayhem.com

Post Reply