[pippin88]

Hello all,

A friend has been generating some gcode via aspire for me.
I had noted that there seemed to be a pause over the area that a tab will be cut deeper down, as the tool moved along a cut.
I had a look at the GCode and aspire is putting in x or y moves that correspond to the tabs even when there is no z move.

For example:
Rectangle cut with 2 tabs along each side on the rectangle (along the X axis)
Tabs 3mm high, 4mm long
Using a 6mm bit
(Unnecessary lines in red)

N470G1X10.125Y10.125Z-9.000F666.0
N480G1X10.125Y145.875Z-9.000F2000.0
N490G1X100.696Y145.875Z-9.000
N500G1X110.446Y145.875Z-9.000
N510G1X636.093Y145.875Z-9.000
N520G1X645.843Y145.875Z-9.000
N530G1X745.875Y145.875Z-9.000
N540G1X745.875Y10.125Z-9.000
N550G1X639.981Y10.125Z-9.000
N560G1X630.231Y10.125Z-9.000
N570G1X114.354Y10.125Z-9.000
N580G1X104.604Y10.125Z-9.000
N590G1X10.125Y10.125Z-9.000
N600G1X10.125Y10.125Z-12.000F666.0
N610G1X10.125Y145.875Z-12.000F2000.0
N620G1X100.696Y145.875Z-12.000
N630G1X100.696Y145.875Z-9.000
N640G1X110.446Y145.875Z-9.000
N650G1X110.446Y145.875Z-12.000F666.0
N660G1X636.093Y145.875Z-12.000F2000.0
N670G1X636.093Y145.875Z-9.000
N680G1X645.843Y145.875Z-9.000
N690G1X645.843Y145.875Z-12.000F666.0
N700G1X745.875Y145.875Z-12.000F2000.0
N710G1X745.875Y10.125Z-12.000
N720G1X639.981Y10.125Z-12.000
N730G1X639.981Y10.125Z-9.000
N740G1X630.231Y10.125Z-9.000
N750G1X630.231Y10.125Z-12.000F666.0
N760G1X114.354Y10.125Z-12.000F2000.0
N770G1X114.354Y10.125Z-9.000
N780G1X104.604Y10.125Z-9.000
N790G1X104.604Y10.125Z-12.000F666.0
N800G1X10.125Y10.125Z-12.000F2000.0
N810G00X10.125Y10.125Z10.000

Is there a setting to avoid this? It's unnecessary code, and does seem to cause a slight tool slow down at these points. (Maybe I just need to fiddle with my Mach3 constant velocity settings?)

Thoughts?

[cutter100]

I think the best bet would be to get in touch with Vectric and see what they say. Although it would kind of suck...you could scan through your code each time and maybe delete the lines?
I have no idea if there's a work around for this. Just out of curiosity how much time does it waste?

[OCNC]

Is there a setting to avoid this? It's unnecessary code, and does seem to cause a slight tool slow down at these points. (Maybe I just need to fiddle with my Mach3 constant velocity settings?)

Thoughts?

If you break the code into two parts you can eliminate this problem.
Part 1: Cut down to the level of the tabs.
Part 2: Cut from the tab level to the bottom of the material.

I have Vcarve Pro 6.5 and this was easy to do. The only wasted move then was going back to clearance height before running the second part. This point is easily located and can be edited out of the code if necessary. The combined files are attached.

Chris

( VectricTest052612 )
( File created: Saturday, May 26, 2012 - 08:12 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 10.000, Y= 8.000, Z= 0.500)
()
(Toolpaths used in this file:)
(Test1a)
(Test1b)
(Tools used in this file: )
(1 = End Mill [0.25 inch])
N110G00G20G17G90G40G49G80
N120G70G91.1
N130T1M06
N140 (End Mill [0.25 inch])
N150G00G43Z0.8000H1
N160S12000M03
N170(Toolpath:- Test1a)
N180()
N190G94
N200X0.0000Y0.0000F100.0
N210G00X1.8477Y1.9597Z0.2000
N220G1Z-0.0938F30.0
N230G2X1.7227Y2.0847I0.0000J0.1250F100.0
N240G1Y5.9495
N250G2X1.8477Y6.0745I0.1250J0.0000
N260G1X7.7077
N270G2X7.8327Y5.9495I0.0000J-0.1250
N280G1Y2.0847
N290G2X7.7077Y1.9597I-0.1250J0.0000
N300G1X1.8477
N310G1Z-0.1875F30.0
N320G2X1.7227Y2.0847I0.0000J0.1250F100.0
N330G1Y5.9495
N340G2X1.8477Y6.0745I0.1250J0.0000
N350G1X7.7077
N360G2X7.8327Y5.9495I0.0000J-0.1250
N370G1Y2.0847
N380G2X7.7077Y1.9597I-0.1250J0.0000
N390G1X1.8477
N400G1Z-0.2813F30.0
N410G2X1.7227Y2.0847I0.0000J0.1250F100.0
N420G1Y5.9495
N430G2X1.8477Y6.0745I0.1250J0.0000
N440G1X7.7077
N450G2X7.8327Y5.9495I0.0000J-0.1250
N460G1Y2.0847
N470G2X7.7077Y1.9597I-0.1250J0.0000
N480G1X1.8477
N490G1Z-0.3750F30.0
N500G2X1.7227Y2.0847I0.0000J0.1250F100.0
N510G1Y5.9495
N520G2X1.8477Y6.0745I0.1250J0.0000
N530G1X7.7077
N540G2X7.8327Y5.9495I0.0000J-0.1250
N550G1Y2.0847
N560G2X7.7077Y1.9597I-0.1250J0.0000
N570G1X1.8477
(COMMENT OUT THE LINE BELOW)
(N580G00Z0.2000)
N590S12000M03
(Test1b)
(COMMENT OUT THE LINE BELOW)
(N620G00X1.8477Y1.9597Z0.2000)
N630G1Z-0.5000F30.0
N640G2X1.7227Y2.0847I0.0000J0.1250F100.0
N650G1Y5.9495
N660G2X1.8477Y6.0745I0.1250J0.0000
N670G1X2.4703
N680G1Z-0.3750
N690G1X3.2203
N700G1Z-0.5000F30.0
N710G1X6.2104F100.0
N720G1Z-0.3750
N730G1X6.9604
N740G1Z-0.5000F30.0
N750G1X7.7077F100.0
N760G2X7.8327Y5.9495I0.0000J-0.1250
N770G1Y2.0847
N780G2X7.7077Y1.9597I-0.1250J0.0000
N790G1X7.0851
N800G1Z-0.3750
N810G1X6.3351
N820G1Z-0.5000F30.0
N830G1X3.2798F100.0
N840G1Z-0.3750
N850G1X2.5298
N860G1Z-0.5000F30.0
N870G1X1.8477F100.0
N880G00Z0.2000
N890G00Z0.8000
N900G00X0.0000Y0.0000
N910M09
N920M30
%

[pippin88]

It's easy enough to do manually, or to do two toolpaths. But really that shouldn't have to be done, the toolpath generation should deal with it.
I might raise it with the Vectric directly.

[ger21]

It's easy enough to do manually, or to do two toolpaths. But really that shouldn't have to be done, the toolpath generation should deal with it.
I might raise it with the Vectric directly.

It has to do with the algorithm that Vectric uses to create the toolpaths. From what I've heard, it would require a lot of work to change.

As you mentioned, try playing with your CV settings to see if you can get Mach3 to ignore them.

[CarveOne]

I don't know if it will help in this instance, but it may be useful to know that when you create closed vectors you can node edit them and move the start point anywhere you want it to be by clicking on an option to change an existing node (black square dot) to a start point (green square dot) or you can add a new node where you want it to be and define it as the start point.

I'm thinking that a start point next to a tab can cause some strange looking moves. May be worth investigating.

[dptp9lf]

Hi,
Have you ever figured this problem out... I'm having the same issue with Aspire and Mach 3. It's just a slight stutter but it affects my cuts
Cheers
Lyle

[pippin88]

I now use LinuxCNC. Aspire 8 I think

I haven't noticed the issue for a long time. However, I tend to use 3D tabs now, which may be different.

[louieatienza]

Check your part too, make sure that section is one straight line, not a cluster of nodes in a straight line... aside from the normal CV settings check the look ahead number, it's default very low like 10 or 20 lines.