Router Forums banner

1 - 20 of 47 Posts

·
Registered
Joined
·
4,352 Posts
Wonder if your Post Processor setting that you changed when you hooked up the tool sensor has anything to do with it??

Since the preview came out ok - but the finished model didn't have the same detail ...........hmmmmmmmmm

HJ
 

·
Registered
Joined
·
1,171 Posts
Did you switch bits between tool paths? Looks like the final pass of the flag the Z touchoff wasn't low enough. Might have been a bit that was loose in the chuck and moved up as it cut.

4D
 

·
Registered
Joined
·
334 Posts
Discussion Starter #7
Did not switch tools. Used 1/8 ballnose. After results lowered bit 1/8 of an inch and reran program and all it did was take 1/8 more material off. Was gone all day to outlaws so will try manual mode tomorrow.
Mark
 

·
Registered
Joined
·
4,352 Posts
I know he changed the Post Processor setting when he installed the tool sensor and the file I sent him was in my PP setting, which doesn't have a tool sensor. Could that be it? That file cuts just like the preview on my machine.

HJ
 

·
Registered
Joined
·
3,724 Posts
The Post Processor is probably the trouble. You need to use the correct 3d PP for your machine.

Some PP are set up to calculate the gcode to smooth out small variances in the vectors from node to node often jumping nodes to smooth the toolpath. When cutting 3d you want to cut all the vector from node to node that the tool can reach so you get all the detail from the model you can get from your tool choice, this is why it takes longer to cut 3d files.

If you use the correct PP when saving the toolpath then you should get a carving that has the detail shown in the preview. If you use the wrong PP for the type of toolpath you are saving then the results will be different than the preview.

You might check with Vectric or the manufacturer of your CNC to see what Post Processors they recommend for your machine.
 

·
Registered
Joined
·
4,352 Posts
Mike,

He has cut things out of files that I sent him before. Then he hooked up the tool sensor and had to change the PP to download the tool sensor file, because I don't have one.

HJ
 

·
Registered
Joined
·
3,724 Posts
I would not think that the tool sensor (touch plate) would have anything to do with the post processor he uses for saving the toolpaths unless he actually changed controller programs so he could use the tool sensor.

If in-fact he changed control panel software then he needs to use the correct post processor for that control software and he needs one for 2d toolpaths and one for 3d toolpaths.

If you had a CNC Shark and decided to change from the Next Wave control panel software to Mach 3 then you would need to change post processors you use so the control software will process the gcode correctly. Each post processor compiles the gcode for a specific program to read, if sent to a different program then the results will be different.
 

·
Registered
Joined
·
3,724 Posts
Mike,

He has cut things out of files that I sent him before. Then he hooked up the tool sensor and had to change the PP to download the tool sensor file, because I don't have one.

HJ
Are you talking about a touch off plate to zero the tool or are you talking about an automatic tool changer to change tools for an entire job?

If it is a touch off plate it should not require any change to the post processor.

If it is a tool changer then it probably would require a different post processor but there should still be post processers for 2d and 3d work.
 

·
Registered
Joined
·
334 Posts
Discussion Starter #14
As the spindle turns update. I reloaded the gcode and used the emc manual mode pp and all worked as normal. Stars and stripes showed up. Eagles feathers are present. I did have to change the pp for the automatic tool length sensor. I am going to try a simple flower with the tool length sensor and see if it works or if it was because John and I designed it in the manual emc mode. I just don't understand how if it works in the preview how it does not work in the post processor that I choose
Mark
 

·
Registered
Joined
·
1,171 Posts
The G64 code in the header section of the Post Processor is probably where the difference lies. The number that follows G64P???? determines how closely the machine will stick to the tool paths. A number of .01 will allow the bit to vary up to .01" from the programmed path in favor of quicker cut times. Reducing that number to .001 will give you a ten-times sharper image as the bit now can not get any farther than .001" from the programmed path. The only "loss" is that the cut may take longer. For the higher degree of accuracy the bit has to slow down more then speed up again as it approaches then leaves each node point.

Codes in the header section of the post processors are Added to the cut file when toolpaths are saved. VCarve or Aspire can't know what codes may lie there, so their preview views are a "best case" that assumes nothing in the post processor will change how the bit moves.

4D
 

·
Registered
Joined
·
334 Posts
Discussion Starter #16
I did notice that p was .010 on auto tool length and .001 on the manual mode. What I don't understand is that when John sent me the files all I did was use the auto tool length sensor and it was at 010. When I set the cut up manually using the emc processor it read 001. I made no changes other than the ppost processor so why did the p number change.
Mark
 

·
Registered
Joined
·
489 Posts
Mark,

The change that you need to make is in the post processor for your tool length sensor (for Vectric software). Read this and maybe it will help you understand. G64 - PROBOTIX :: wiki

It appears that your "manual" post processor has a G64 P0.001 tolerance and the Probotix LinuxCNC AtLas G64 Arc Inch TTS.pp has a G64 P0.01 tolerance. If you change it in the post processor to G64 P0.001, you will never have to worry about it again.

If you can't figure out how to change it, send me a email and I will send you the change file.

Here is a snippet of the PP file:

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"%"
"(PROBOTIX LinuxCNC)"
"G0 G54 G17 G20 G90 G40 G49 G64 P0.010"
" "
"o100 CALL [91][T][93]"
" "
"G0 [ZH]"
"G0 M3 M8 "
 

·
Registered
Joined
·
334 Posts
Discussion Starter #18
Do i change it in the aspire program or on the computer that runs my nebula. I have never programmed or changed anything for my cuts so far because the manual has already been working. I read the links and understand why I need to change the p numbers but the links don't say how or where.
Mark
 

·
Registered
Joined
·
489 Posts
Mark,

Open Aspire, go to File > Open Application Data Folder... >PostP.

Find the post processor file for your tool sensor (Probotix LinuxCNC ATLas G64 Arc Inch TTS). Open the file and scroll down until you find the 'Header' section, change G64 P0.01 to G64 P0.001. Save and exit.

Restart Aspire. Now when you choose this pp, it will have the tolerance of .001.

When you are in the Application Folder location, you will see a folder named 'My_PostP'. This is a special folder that you can add just the post processor files that you normally use. Then in Aspire when you go to choose the PP to save your toolpath with, you will only have the ones you use, instead of the whole list. I find this very useful. I have copied, renamed pp in this folder with different tolerances. That way if you don't need 0.001, you can choose .01 or whatever.

Let me know if you have any other questions.

Dave
 
1 - 20 of 47 Posts
Top