# Results do not match 3d preview



## edison auto (Nov 13, 2015)

Tried carving eagle and flag. Preview is perfect no stars or feathers. Any ideas. 
Mark


----------



## OPG3 (Jan 9, 2011)

Antecedent, please.

Otis Guillebeau from Auburn, Georgia


----------



## honesttjohn (Feb 17, 2015)

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


----------



## edison auto (Nov 13, 2015)

Going to try !manual mode tomorrow. Here is pic of preview


----------



## edison auto (Nov 13, 2015)

Here is pic of cut still on table


----------



## 4DThinker (Feb 16, 2014)

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


----------



## edison auto (Nov 13, 2015)

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


----------



## honesttjohn (Feb 17, 2015)

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


----------



## MEBCWD (Jan 14, 2012)

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.


----------



## honesttjohn (Feb 17, 2015)

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


----------



## MEBCWD (Jan 14, 2012)

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.


----------



## SteveMI (May 29, 2011)

If from vcarve, it looks like the roughing toolpath only before finishing toolpath. 

Steve.


----------



## MEBCWD (Jan 14, 2012)

honesttjohn said:


> 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.


----------



## edison auto (Nov 13, 2015)

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


----------



## 4DThinker (Feb 16, 2014)

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


----------



## edison auto (Nov 13, 2015)

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


----------



## beltramidave (Jan 6, 2016)

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 "


----------



## edison auto (Nov 13, 2015)

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


----------



## beltramidave (Jan 6, 2016)

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


----------



## beltramidave (Jan 6, 2016)

see attachment


----------



## edison auto (Nov 13, 2015)

Thanks dave for the help. I will go home tonight and change it. So as far as the list goes if i just add the linux and the manual one that i have been using to my postp and those will be the only 2 there is that correct. What is the normal time difference between the 001 and 01. I know it will vary depending on the degree of detail but on something like this eagle if it is only 30-60 minutes longer why mess with different pp settings. Maybe because mine is still a hobby and not a money maker time does not matter. Or maybe if i am understanding it correctly i would use the 01 for vcarving and the 001 for 3d carving.
Mark


----------



## beltramidave (Jan 6, 2016)

Make sure to put them in the "My_PostP' folder if you only want those to show up. Like I said you can set up multiple files and only change the tolerance if that is what you want.

As far as when to use a smaller tolerance, you are correct. Normal Vcarving and profiling cuts would work fine with G64 P0.01, but if you want good detail in your 3D work, you are going to want G64 P0.001 at minimum.

I just pulled this one off the machine this morning. Total size is 4.5Wx3.5H.

Dave


----------



## cjskelton (Feb 27, 2015)

Dave, what size bit did you use to carve your project? It looks great.

Jay


----------



## edison auto (Nov 13, 2015)

Dave I got the pp setup and my files are setup and ready to use. I am going to try some tomorrow night. Thanks so much for the help from you, John and Mike and everyone else. No one can do all of this by themselves. Like i said on another post woodworkers helping woodworkers. Once again thanks
Mark


----------



## beltramidave (Jan 6, 2016)

Thanks Jay. 

For the fish, I used a .25" diameter 30 degree V bit with a .01 flat tip. The texture was done with a .25" ball nose.


----------



## honesttjohn (Feb 17, 2015)

I just pulled this one off the machine this morning. Total size is 4.5Wx3.5H.

Dave[/QUOTE]

Is that inches or feet??? That would make a heck of a large wall panel!

Did you run the Vcarve bit in 3d finish toolpath?

HJ


----------



## cjskelton (Feb 27, 2015)

I was thinking the same thing, HJ. A V-bit was used to cut a 3D model ?? What!! I guess I have a LOT to learn in this hobby.

Jay


----------



## honesttjohn (Feb 17, 2015)

You and me both, Jay

HJ


----------



## MEBCWD (Jan 14, 2012)

Jay you can use all kinds of bits for 3d work but some are a lot better than others. I have one heart in my jewelry line that I use a 45deg v-bit, no flat tip, just so I could get a little bit of texture on the face and it workes great with a around a 5% step over. The best bits have the smallest tip so they can get the finer detail in the model but take the longest time. Sometimes on models with out fine detail you can get good detail with a larger bit and save a lot of time. Other times you can save time by using a larger bit to cut most of the project then come back with a smaller bit and just cut the fine details, this is called Rest Machineing.


----------



## beltramidave (Jan 6, 2016)

That would be in inches, lol. Would love to make something that large with that much detail.
I learned the flat tip vbit trick from a guy on the Vectric forum. We all have a lot to learn, that is what makes these forums so great!

Yes, HJ, it was only a finishing toolpath.

Dave


----------



## honesttjohn (Feb 17, 2015)

I got a 1/16 ball nose -- that would have done just about the same, wouldn't it?

What do I need to engrave bronze plaques?

HJ


----------



## beltramidave (Jan 6, 2016)

Sorry John, doubt a 1/16" (.0625) ballnose would do the same as .01 flat. I have a 1/32" tapered ball nose, that wouldn't do it either...at least at that size.

Plug those tools into your Vectric software and do a preview to verify. I used a .005 stepover.

Here is the finished piece. Have no idea what I am going to do with it as it was just a test piece.

Dave


----------



## cjskelton (Feb 27, 2015)

Here is a test cut using a 1/8" ball nose bit in a 1" thick piece of cypress. Looks better now that I've changed the G64 setting. Dave, your's looks incredible. How long did it take to cut with that tiny bit?










Jay


----------



## beltramidave (Jan 6, 2016)

Took a little over 2 hours. Had speed set @ 125IPM on both feed and plunge, but never made it over 60. It's not a fast process, but the results were good.


----------



## honesttjohn (Feb 17, 2015)

Jay,

Did you get the tool length sensor?

HJ


----------



## cjskelton (Feb 27, 2015)

My Meteor came with the tool length sensor. I'm thinking of getting the Z-Puck, though. That would take the work out of zeroing the Z axis. 

Jay


----------



## honesttjohn (Feb 17, 2015)

If you get the Z-puck then you don't need the sensor??

HJ


----------



## cjskelton (Feb 27, 2015)

You use the Z-Puck to do the first Z-axis touch off then the tool sensor adjusts Z with each bit change. Saves manually doing the first Z touch off. It should make the touch off faster and more consistent.

Jay


----------



## cjskelton (Feb 27, 2015)

I ordered the Z-Puck today. Len says they are working on a new, streamlined LinuxCNC control panel (GUI) that is less complicated. The current version will be for the 'Power User'. On their Wiki is a new LinuxCNC configuration that adds some new features including the touch off puck.


----------



## beltramidave (Jan 6, 2016)

You are going to like the Z puck. I had made a touch off plate about 1-1/2 years ago as I got tired of trying to jog down to the top of the material with any repeat-ability and accuracy. It actually doubles as my tool sensor too - same input for me. Works slick!


----------



## honesttjohn (Feb 17, 2015)

So if I get the Z puck I don't need the tool sensor? Just want to get this right.

Also looking at their stands. My Nebula is on a homeade table. Wonder if that's part of my leveling problems.

HJ


----------



## beltramidave (Jan 6, 2016)

John,

The tool sensor and the Z puck serve 2 different but similar tasks. You always have to zero your Z axis either to the material or table (using the Z puck or manually). The difference is that if you have the tool sensor, you only have to zero your Z axis once. So if you are running a job with multiple tool changes on the same part, you put a tool in your spindle and Linuxcnc will measure the tool using the tool sensor. Then with the same tool in the spindle, you use the Z puck and touch off on your material. When you create your toolpaths in Vectric, you give each tool a specific number and when you save your toolpaths (using the correct post processor), Vectric will auto-magically stop your program when a tool change is needed. You then change the tool and the program will auto-magically position your new tool over the tool sensor and touch off (calculating the new tool height) and the program will continue until the next tool change or program end.

If you are strictly running toolpaths with no tool changes, then the tool sensor would not be needed.

Hope this makes sense.

Dave


----------



## edison auto (Nov 13, 2015)

John that is what i was talking about having my tool sensor working now i do not have to reset my z axis when i change bits. It makes it easier especially when doing carvings. Now that i got the right post processor i am going to run the doves this weekend and see how they turn out. If all goes well I will order the zpuck just to make things easier. As far as your table goes when I was building my table I took some cues from 4d and built my legs out of 4x4 cypress with 2x6 frame work. The entire table is on wheels and i have not put the casters down yet. I leave the table mobile and even move it while it is carving. If i remeber correctly when I was talking to len about the table he said it does not have to be level as long as all 4 corners are on the same plane. Theoretically you could mount it on a wall as long as the gantry would move or have 1 end 3 inches lower than the other end as long as everything is flat. Side to side would be more of an issue as the gantry might bind if 1 side is lower when you bolted the machine down if I remember our conversation correctly. I have found the center of my bed is 2 playing cards .019 low in the middle in between my bed supports. At my bed supports all is level and at both outer edges all is good. As a technician and a machinist i tend to get numbers pretty small. I am not sure .019 is enough to worry about on most things. Just my 1 cent worth(haven't done enough carvings to have 2 cents worth. lol)
Mark


----------



## beltramidave (Jan 6, 2016)

Mark or John,

What did you do with your computer, monitor and controller? I need to make a stand of some sort for my revised machine. I want to make it mobile as well as my machine has a moving table with a fixed gantry. So there are times I would need to move it away from a wall to allow machining of longer parts or feed thru. Would like to enclose computer and controller and maybe use a furnace filter or something to allow air flow.

Need ideas..

Dave


----------



## honesttjohn (Feb 17, 2015)

Mark,

My machine is just sitting on a table - not bolted down.



Dave,

I have a short table that slides under the main table. The only thing I have to move if I slid it under would be the monitor. There's really no easy space efficient way I've seen yet, especially if you're short on room. Was doing some thinking when I saw a small portable kitchen island at Wally World. Chrome top, drawer, shelf, on wheels, cheap....... 

HJ


----------



## edison auto (Nov 13, 2015)

My computer and all is on my desk right now. I am adding a swing arm and a slide out for the monitor and mouse. The computer and controller will sit under my drawer on opposite end of stop switch.
Mark


----------



## beltramidave (Jan 6, 2016)

Looks good. Like the drawer idea.


----------

