photo v carve post processor

[large519]

Hi, When I post a toolpath from photo carve, the plunge feed rate is not shown in the programme??? Only the cutting feedrate is shown, I use an edited copy for both my router and mill, and they both miss the same Feed rate, I have also tried using different pp's for different machines but they all come out the same,
The setup is set to mm's, feedrate of 1500 and plunge rate of 500. Only 1500 is shown in programme?
Any helpful advice much appreciated

[Adrian]

Do you mean the plunge rate is not being shown in your controller software or it's not in the actual code that is saved?

The plunge rate is show in my ShopBot files correctly when using PhotoVcarve. Which PP's have you tried?

[large519]

It's not being shown in the actual save g code programme. I'll post a copy of the saved programme and the pp used.

[large519]

This is a copy of the final saved programme - only showing a plunge and feed rate of F1500.

Router1example.txt

(706 Bytes) Downloaded 320 times

This is the router PP that I editied, I only changed the start and end parts of the programme.

Denford_mm - Routerpvc.pp

(2.76 KiB) Downloaded 280 times

I also tried these standard PP's that are supplied with PVC-
DENFORD_MM
MACH2_3_MM
And these came out the same.

[Adrian]

Not sure why there are no plunge rates in those PP's. Have a look at the "CNCShark-USB (mm) (*.tap)" for one that has plunge rates. You should be able to see which commands you need to add to your PP from there.

[PaulRowntree]

As a test, try replacing the line (#34)

VAR FEED_RATE = [F|C| F|1.1]

with

VAR FEED_RATE = [F|A| F|1.1]

Not sure why this would be needed, but it should put the feedrate on all lines.

It looks like line#90, normal moves, never outputs the feed. Odd (to me)

begin FEED_MOVE

"[X][Y][Z]"

Would
begin FEED_MOVE

"[X][Y][Z][F]"

work?

[large519]

Thanx guys, i'll give your ideas ago. Keep you posted

[large519]

Well, I tried but with no success.

Not sure why there are no plunge rates in those PP's. Have a look at the "CNCShark-USB (mm) (*.tap)" for one that has plunge rates. You should be able to see which commands you need to add to your PP from there.

Adrian, tried the CNCShark, but the tool path was still missing the plunge feed rate.

Paul, didnt get to try your theory.

I decided to uninstall, and re install the software.......and not use my edited PP's, and use the re installed PP's, but...... STILL no plunge feed rate, i used the denford,mach and CNCshark PP's all in mm's.

[Adrian]

I suppose I should have actually checked the output rather than going just by the code. Sorry about that.

Turns out that PhotoVCarve itself doesn't actually use the plunge move section so it's nothing to do with the PP's after all (I even posted in that thread but it was a long time and several brain cells ago....) - http://forum.vectric.com/viewtopic.php? ... 10&p=49518

Because of the way the ShopBot code/controller works the plunge rate does work for me as the (X,Y),Z speeds are independent.

[large519]

[/quote]Because PhotoVCarve was originally developed for the photo-groove machining,
the cutter needed to retract to the Rapid Clearance Gap at the end of each pass
to ensure it can move safely to the next groove without marking the material surface.
When this code was written we decided that this wasn't a time critical process and
decided to leave all moves at the specified feedrate and not include rapid rate retract
and plunge rate moves. This approach means the tool moves from the clearance height
down to the appropriate Z depth at feedrate and not plunge rate. We will look at
improving this for future versions - no time scale at the moment.

Toolpaths calculated in Aspire are standard 3D model machining toolpaths that link
the raster passes together running over the surface and not retracting above the
material. So these toolpaths don't include the plunge moves being seen in the
PhotoVCarve toolpaths.[/quote]

After reading the mentioned string, I now see that the plunge rate will never work, so why put the option in?? and the string was dated 5yrs ago, has this not been looked at since then?

I have already done some photo engraving on wood, using a V cutter, and I didn't notice the plunge rate missing in the beginning, as I had done that piece on my mill which only runs at a max of 450mm/m and a v cutter feeding in at that speed is nothing, but where as I was running test paths on my router, and trying some acrylic (like creating lithoplanes) and using a 1Bn, that's when I noticed the plunge rate missing, and I wasn't keen on the 1Bn plunging in at 1500mm/m. Im sure it would be ok, but I would prefer to have the option.

Would the PP, that I use from Aspire work in PVC??

[Adrian]

No. PhotoVCarve is a much older program and the PP's in Aspire have facilities that the PhotoVCarve would not recognise.

It's PhotoVCarve itself that does not output the section as far as I can see so there's nothing you can really do with the PP's I think.

Aspire can do everything that PhotoVCarve can so you could just use that instead -

Photo line engraving - http://forum.vectric.com/viewtopic.php?f=28&t=8731
Lithopanes (F04) - http://support.vectric.com/tut-aspire-3d-techniques

[large519]

Ok cool, I'll look into using aspire aswell
Thanx for the advice Adrian, much appreciated.