Post processor for Isel .ncp

[Anonymous]

Hi there,

I am looking for some help with an Isel post processor file.

I have successfully modified the scaling from Micrometers to mm which has enabled some workable outputs but I still get frequent errors that I am manually removing from the programs in the machine control. I generally have to remove the first 5 or 6 lines or code from the program, start the spindle manually and then the program will run following the co-ordinates without issue in most, but not all, cases.

The machine is an Isel, Flatcom M40 and controller (i believe) iMD 40 CAN (info can be found at the following link) https://www.isel.com/hu/downloads/dl/file/id/4230/technical_ordering_data_imd10_20_40.pdf

Any help gratefully received, I think that the supplied post processor is nearly there but just have no idea how to modify it any further.

(I will add some samples of the generated programs when at work tomorrow morning)

Thanks
Ben

I have attached 3 files (files too big to attach so compressed in a .zip) that I have run, supplied is a little info on each:

Test 1.ncp
A simple test in 3D with an 3D adaptive clearing cycle and a contour finishing pass.
This test worked file after removing lines N20 to N70 (also removed on all subsequent programs), although an error code appears on the spindle start although the spindle still starts up.

Test 2.ncp
The adaptive clearing worked fine on this example however the parallel finishing pass would move small amounts then throw up an "unexpected co-ordinate error" although if I forced the program to continue the toolpath continued as expected, but it would continually throw up an the same errors 10 or 15 times per pass.

Test 3
This is an example of another issue that reoccurs throughout all the programs that include pocket cycles. The tool cutter hangs over the work piece and tracks around in small circles (x,y) movements for minutes at a time before then plunging in to complete the pocket operation. See section N170 to N9070 for the first example of this in this code.

Also attached is the .cps file that we are using.

[Anonymous]

Hi Ben

I have also isel machine, like I have written in the post below I am almost there with changing isel post file. In my case erros in the first few lines were WPCLEAR and SPINDLE ON. WPCLEAR commands machine to whipe zero coordinates - I've deleted this line. Try deleting "ON" in line with spindle to turn it automaticly. It should look like this:
N45 SPINDLE CW RPM13926
You can try my modified isel.cps maybe it will get you closer to error free post.

If you still have errors, pls write more specific.

EDIT:
Ben, I saw that you edited your post during my reply. I am not programmer of any kind, I modified isel file with logic and reading, so I don't know if I can help you more. One thing I noticed that my machine freezes when circular interpolation is to small, it can occour specialy when finising passes are very precise. When you post file try to change setting minimumCircularRadius to 1 or above, it could help.
Just for a test delete line that says:
allowedCircularPlanes = undefined; // allow any circular motion

this would not allow your postprocesor to write any circular interpolation (bad for machining time). If machine wouldn't state an error that would be your issue.

[Anonymous]

Thanks very much for the info, I have compared the post processor files and can see where you have modified it. I was thinking about making some similar changes but wasn't sure where to start.

I will run a test with your post processor and try out some of your other suggestions.

I'll post the results back up here.

Thanks again

[hai.cao]

TheMasterpimpek,
  thanks for uploaded your isel post ; )

Ben,
  If the post processor needs further edits, please upload the marked up changes needed.  We will customize the post for you

[Ansunist]

Hi
I have been a solidwork/camwork user before and  I am still a rookie in 3D software.
I have started with Fusion some days ago and have tried to get a hole though to my light CNC machine

I have Isel ICP 4030 with a 3D Kay module from Galaad. The Kay module accept the isel generic .ncp file, but it seems that the kay module misunderstand something, please see the udklip. Please also take a look on CNCcode. The size of the part is far to big 😞

Hope somebody can help

Br Ansunist

[Machiel-Hulsman]

Hello Ansunist,

I've got the same machine (ISEL ICP3020 in my case, including the KAY upgrade). I had troubles as well so I made changes to the ISEL post processor in Autodesk. My machine would begin with going to Z=0 and then up 0,5mm and then begin work... I fixed this by blocking out (in the lines 341 and 342):

writeBlock("FASTABS", zOutput.format(toUM(machineConfiguration.getRetractPlane()))); // retract
zOutput.reset();

The other (first 😉 )change I made was to set the processor from micrometers to millimeters:

/** Returns the feed in mm/s. */
function toVel(feed) {
  return feed/60 * 1000;
}

/** Returns the spatial coordinate in millimeters. */
function toUM(spatial) {
  return spatial * 1000;

Now it runs fine, except for one issue. After (at the end of) having milled a circle, the mill will first dig down for another 0.1mm before going to the next operation, thus ruining my work... still working on this one. Spline systems is helping me out on this, they luckily have great service!

Hope this helps yet another bit. I attached my post processor (as txt).
If you are interested in Spline's solution, I can let you know as well. Good luck!

[Ansunist]

Hi Machiel-Hulsman

really appreciate that 🙂 
I have already tried your post and its looks much better. I have some issues regarding the adaptive milling where its like the plunge feed rate is to low.
If you get a solution for the Kay issue I will be happy to hear from you again.

Br André

[Ansunist]

Hi
I have Isel ICP 4030 (Axemotion) with a 3D Kay module from Galaad.

My Kay simulation of the adaptive clearing also show that the tool make small circles for 4-7 min before its plunge down in the stock.
Any ideas to modifications in the post ?
Br André

[Machiel-Hulsman]

Hi Ansunist,

I attached my latest post processor with another update regarding the strange drop at the end of milling a circle.

Regarding the small circles, did yuo check the ramp (in the Linking tab)? Maybe you've set it to 'Smooth profile' or 'Helix'.

The feedrates (for plunging as well) can all be set independently, so that should fix that problem.
)I also noticed that Sideways compenstaion is set to Left by standard, I've set mine to Right (conventional milling) for a better result).

Another 'step' forward? 😉

[Anonymous]

Hi all,

I have been meaning to post this back up here for a little while...

I am running this post processor with no problems on ISEL Flatcom M40, the only small issue is that the program code starts from the datum point at Z0. I manually raise the Z to just above the work piece after setting the datum point.

The helix plunge does seem to lower quite slowly but no longer hangs in the air for lengthy periods.

We use the machine as a simple 3D router with no tool changer or coolant so both are disabled in the post.

I'm no programmer but have modified the post through trial and error and picking up some tips here and there.

Hope it may help somebody.

Ben

[Ansunist]

Hi
I have tried the post from Machiel-Hulsman, thanks.
It´s seems that the small circle after the facing have eliminated :). The ramp isues is also solved due to your advice.
It still doing some testing and there is some problems with 2D adative clearing. I hope I can find a way around.
Br André

[Machiel-Hulsman]

Seems like we´re getting there slowly but surely 🙂

Please keep us posted with any findings and/or changes concerning the post processor (I will do so for sure).

[Ansunist]

Hi

The ramp issue is unfortunately still present. When I trey to make a circular hole,  the tool makes a number (number of treads?) of circular movements in the same plane, before it moves fast down:-(

The machine c'ant keep the the work-piece z-zero, when I change tools. It moves the work-piece around 50 mm downwards, which results in a broken tool:-(

Thanks in advance

André

[Ansunist]

Hi
I have simplified the geometry, just a hole in plate. It looks like the Fusion generated path is fine. After the post processing the Kay picture shows that the post is the problem.

Br André

[Ansunist]

Hi Thanks for the help with the new post. I have still a facemilling issue. The postprocessor will generate a toolpath with some large radius arc. Please take a look on the attachments. When I inspect in Owein I cant se the circles ? br André

[Ansunist]

Hi Thanks for the help with the new post. I have still a facemilling issue. The postprocessor will generate a toolpath with some large radius arc. Please take a look on the attachments. When I inspect in Owein I cant se the circles ? br André

[Ansunist]

the attachment

[Anonymous]

Hi 2 all 😉

i'm working with a ISEL ICV4030 and have a little trouble with the feedrate.

no matter what i adjust in the inventor - the post porcessor overrites it and feeds the Mill with 120mm/sec instead of the max of 8mm/sec...

is there any idea for modification the post processor that he does not overrite the speed of the feadrate? (without making everything besides that slow 😉

thanks in advance!

[AchimN]

Thanks for all your feedback.

FYI, we are working right now on the generic isel post processor, so there will be improvements soon.

The updated post will show up into the post library:

http://cam.autodesk.com/posts/?p=isel