Converting Aspire files for rotary output

Converting Aspire files for rotary output

Postby gravirozo » Tue Sep 08, 2009 3:13 am

hello all

today i downloaded the wrapper, but however my gcode file could be too large so i could not convert....

i wanted to find out the reason, for "converting angles" and find out why the circular interpolation doesn't work in rotary mode...

first here's a drawing as a shape get "wrapped"..... as you can see, the horizontal lines will lay on a diameter and, in this case the vertical lines on a straight line from center to any point on perimeter...

so,,, the point was in rotary mode "must to be" in angle...
what is in "flat" version staraight, horizontal that laying on a circle... in flat mode the x or y axis will move, just for example 100 step on one segment...
in rotary mode you can set also 100 step....
also you can say mach it is not 20 mm but it's 20 deg...
so,,, here's the trick...

this drawing 360 mm long... so the dia meter around120 mm approximately, but if you set the secondary axis for angle, or A axis mach will say one unit is one degree...
but this drawing also can be used as "swapped axis" just simply using the Y settings on the rotery...

when you use the Y axis with pinout A then mach will count on this as "flat" and drive the A axis as it would be Y...
really doesn't matter the speed, since the bit tip in any mode spinning with a predefined rpm

the backlash... you can say angle, and mach convert it for step... for example 15 step on one turn...
also you can say you need the 200 mm diameter and on this diameter the mm will be converted same 15 step....

when you mill the top that is 20 mm, and the bottom also "20 mm" but that is wirtual 20 mm already... same quantity of step will describe like the outer...

also a point the feed is changing... yes in this case it will drop as get closer to the center.. IF it is going on the perimeter... if it is going lenghtwise, then the X and Z axis will define the feedrate, what is controlled...and the agularspeed of feed has affect only when passes are shifting on the passes end...

so without i know how they program works... i used fully aspire to generate the gcode... direct output from aspire...
the "converting" what is actually resizing the drawing in X or Y direction to 360 unit with aspire takes about a few seconds...

to write out a toolpath also not a lot time...

the cutoff of the postprocessor made after brian's instruction... from the pp editor manual... the home position will write out "normal" Y position while the positions in feed will be written to A or any letter you like...

thanks
viktor
Attachments
basics.jpg
swapping letters.jpg
gravirozo
VCarve Wizard
 
Posts: 1983
Joined: Sat Jan 10, 2009 12:38 am

Re: rotary output from aspire

Postby gravirozo » Tue Sep 08, 2009 3:21 am

hello all

also i have some test files...
i made in aspire, using a very simple geometry.... one of them i plan to "decorate" with grapes, other will be itself an ornament...
this way we can make some extra ornament on the twisted surfaces...



yes, goldner's indexer can make easy a rope or any twisted form... also in case a series, that works faster with a profile bit...


how ever there are some limitation... for different leads might need different shaped tool what is not a cheap stuff... with this method a simple ballend mill do all profile...

thanks
viktor

the gcode output was displayed with gcode editor... this was my worst point, i could not show the wrapped output...
Attachments
base for grape post.jpg
material settings.jpg
rope post in aspire.jpg
rope post.jpg
gravirozo
VCarve Wizard
 
Posts: 1983
Joined: Sat Jan 10, 2009 12:38 am

Re: rotary output from aspire

Postby ManitobaKeith » Tue Sep 08, 2009 4:01 am

Viktor,
Wrapper 1 is quite slow. If you start the conversion and wait, it will complete.
I tried a REAL 3D file with over 575,000 lines of code using Version 2 Beta, and it converted in less than 5 seconds. I think it took 15 minutes in Version 1, so it is a huge speed increase. One other thing I have heard is that there is no 3D arc output by Aspire or V-carve and Mach3 is not capable of arcs. So, what's the big deal with arcs - I don't know a lot, so please explain. Is arcs like Y2K? I have also heard from people that have WinCNC and they are using Wrapper.

If you can PM send me the file that you had trouble converting, I will convert it for you and send it back to you.
Keith
It is not only what we do,but also what we do not do,for which we are accountable-Jean Moliere
User avatar
ManitobaKeith
VCarve Wizard
 
Posts: 374
Joined: Sun May 03, 2009 2:06 am
Location: Noble Lake, Manitoba Canada

Re: rotary output from aspire

Postby gravirozo » Tue Sep 08, 2009 4:20 am

hello keith


i have no doubt both program are great... next files i will try... however i made them directly from aspire and they using "angle"....
it's only an option... just like those program... i may make a small file... but i was really tired, i worked daytime on the roof... so i just wanted sit dow :-)


thank you to offer your help...

viktor

the g arc can be a thread or similar... but in case wood, and with CV not really important
gravirozo
VCarve Wizard
 
Posts: 1983
Joined: Sat Jan 10, 2009 12:38 am

Re: rotary output from aspire

Postby Greolt » Tue Sep 08, 2009 5:11 am

ManitobaKeith wrote:One other thing I have heard is that there is no 3D arc output by Aspire or V-carve and Mach3 is not capable of arcs. So, what's the big deal with arcs - I don't know a lot, so please explain.

Keith

There is a lot of misconception about arcs. And when I say arcs I mean G2 an G3 commands. Where the controller (Mach3, WinCNC, Fanuc etc.) interpolates an arc movement from a set of gcode command parameters.

Aspire and Vcarve Pro can most certainly output G2 and G3 commands in gcode but only in 2D toolpaths. Not in vee-carving or 3D.

I think what confuses people is that the post processor that they use says "arcs" as part of it's description.

What that means is that post processor will post G2 an G3 moves where appropriate only in a 2D toolpath.

If a non arc post processor is used, then even 2D toolpaths will contain no G2 or G3 commands. They will automatically be segmented.

As far as Mach3 is concerned, like all controllers that run gcode, it does not interpolate arcs on a rotary axis. A, B or C.

The issue is not that wrapping has introduced this limitation. It is built into gcode. It is already there. It is industry standard.

Mach3 does use G2 and G3 movements in a flat plane. X-Y, X-Z or Y-Z. As do most other gcode capable controllers.

The important part of all that is, that in rotary axis work that we do with our 4th axis, the gcode that we use will for the most part will contain no arcs.

And for the very rare occasions (I can not think of an example) that 2D toolpaths are used with arcs then segmented code will make no or little difference.

Hope that makes it clearer.

Greg
Greolt
VCarve Wizard
 
Posts: 840
Joined: Fri Sep 21, 2007 1:44 pm
Location: Australia

Re: rotary output from aspire

Postby gravirozo » Wed Sep 09, 2009 9:39 am

hello all


in this post i try to show the logic of rotarywork...


my life is flipped over a little in the recent weeks... i try to make my building for store, and almost every day i have to go on some job... tonight we installed some interior doors, and baseboards in a new house... i just got back around 2 oclock night...

so...

what i find out about rotary...greg gave the solution when he stated ""because it is dead easy"""
yes it is...

when you use in normal way a rotary axis, the controller, wincnc, mach, turbocnc or any... expect angles... does mean your stuff must correspodence with this...

what does it mean...

in a sample drawing, i made with cut2d... used 360x360 mm drawing...

this will be a full circle...nothing about diameter... so the drawing what you would like to put on a cilynder need to be match with 360... on the axis you want to wrap...

let see the test...

i made a simple profile toolpath with on option and saved toolpath with mach postprocessor... i could use any of postprocessor...
only changing the variables, for Y cordinate will be written A, but home position not written over...
so the machine run in homeposition as x y z, with feed run to the position and axis will be driven from here A X and Z

on the end of task will be run back to homeposition...

the diameter will be set with material thickness... in this sample i did set material 50 mm and zeropoint is the material bottom...

if you set for different thickness then that value will be the radius of your project...
by 360 value it will ru a full circle...

on following post i try to show how you can set your drawing for a diameter, or how you can make only part of a full circle...


thanks
viktor



i choosed cut2d, because it is a "cheap" program... however this little program able to generate a rotary toolpath... just like cad-cam programs... different way, but result is same...
Attachments
cut2d 2d view.jpg
cut2d preview.jpg
setting diameter.jpg
in editor.jpg
gravirozo
VCarve Wizard
 
Posts: 1983
Joined: Sat Jan 10, 2009 12:38 am

Re: Converting Aspire files for rotary output

Postby gravirozo » Tue Sep 15, 2009 5:14 am

hello all


since few weeks i just wrestling with my junky shed, and try to get ready an another one....

today i made some experiment to find out more about fourth axis... in first sight i wanted only swap axises, however i was unable to set mach for this... so i had to choose "converting" to angles... what is not really true, however mach sensing as they are angles...
i had some discussion with greg and he pointed out in inches the different between 360 and the values too high...
also the preview very important before cut... the backlash will work on any way... mach associate backlash to steps independently you set any unit (miles, liter or meter) in rotary mode mach limiting the work area to 360 unit just like a clock, after 12 coming the one... all directionchanging will result a backlashcorrection on actual axis, valued as preset...


so first i looked around in mach what i could set... on the x-y-z axis available simple resizing-scaling... this option not showing for A or 4th axis... however machsupport said over phone there's the G51 that can do that with axis name and with parameter as the scaling value...

my interesting was on fact as aspire makes 6-8 mb pure gcode less than a minute... mach also run trough on 6-10 meg file less than half min... so they might able to make me this little calculation...

so here's my first test...
in this example guessing i have a post rounded for 72.8mm diameter, and setting on 3 of anjou lily around between 10 mm gap...from vectorart3d site... and all made with free machinist... as everyone can test this, with download that program...

ie many user has no aspire or vcarvepro...

first i made changes in the postprocessor... it made for mach, but the g51 code works in wincnc too... about shopbot i have no too much info as it use some special codes...
in the beginning of the PP in the define variables part, i made changing on Y axis, as it gives A letter inpositions, in homeposition use Y letters, in movement, and rapid use A letters...

before all movement i inserted the G51 code with A letter and a scaleing value... this value came from
""" 360 / diameter x "pi" """" equivalency...
360/ (72.8 x 3.14526) this is the scaling value, as picture need to be "stretched"
in this sample i set manually... however the postprocessor can be set as this value will be read out from the partsize... as it is a real variable in vectric programs


IMPORTANT IF YOU TURN ON AND SET G51 VALUE DIFFERENT AS 1.000, THEN YOU NEED TO TURN IT OFF ON END OF GCODE
BECAUSE THE SETTING WILL REMAIN AND ON NEXT TASK IT MAY OVERWRAP


so i have 228.974 lenght for three model plus 3x 10 mm gap.... equal 3x 66.3249 plus 10 mm

made toolpath in machinist with zero start on lower left corner, set material thickness for 36.4 and zero on the material bottom... recalculate twice, with 76.3249 and 152.6498 offset-shift for zeropoint...

the three toolpath unified-merged in notepad... wordpad leaves some unwanted characters that you can't see...

loaded in mach....

the result is, with free machinist we already could wrap some 3d models... the mach preview just proof it is working.... alsoneed a third party program, notepad...


thanks
viktor
Attachments
settings for diameter.jpg
settings for model.jpg
shifting w 76_32.jpg
in mach.jpg
rotary_mm.pp
(2.88 KiB) Downloaded 210 times
3pattern.txt
(25.88 KiB) Downloaded 179 times
gravirozo
VCarve Wizard
 
Posts: 1983
Joined: Sat Jan 10, 2009 12:38 am


Return to Hardware related questions

Who is online

Users browsing this forum: No registered users and 1 guest