Post processor for Weihong NK105 (Solved!)

[Anonymous]

This is all completely new to me so excuse me if I get something completely wrong. Please enlighten me I'm very interested in learning.

The post processor in question is for a custom made 3 axis CNC router from China with Weihong NK105 controller. I have found a few posts on various forums on this topic but all a bit vague and with no reference to a positive outcome.
From the searches I have done it seems that the fanuc.cps configuration is the one to start off with. It does indeed work. I have only done some preliminary short runs and all seems well except I get a G94 error. The controller skips past it and completes the run with no further problems. This makes me think my feed speeds are being ignored or perhaps wrong.

Before I dive into this any deeper I am sure there are others with the Weihong controllers that have come across needing a post processor specifically for this. Can the team perhaps dig out some files and send to me for test? I am thinking this might be easier than to debug everything from scratch with the fanuc settings.

One other small annoyance. The fanuc.cps demands a number as the filename however the Weihong is perfectly happy with the more human friendly letters and words 😉

Link to the NK105G3
http://en.weihong.com.cn/products_detail/&productId=30.html

Thanks!
/Mark

[skidsolo]

He is a post that was made for the Weihong Studio software.

[Anonymous]

Bingo!
That just works. Thank you.

Mark

[Anonymous]

I am using this post, but the router does not stop on tool changes. It stops now and asks for the next tool. I have no ATC although the machine would support it. Is there an option in this post to have the pause on tool change in a position that is comfortable? The machine also offers a tool sensor, which should be used to measure the new tool. How can I force this?

I also feel like the feedrate is not as slow as set in fusion, causing my tools to break.It seems like the machine does not read the feedrate. You can set the feedrate in 10% increments on the handheld control

[Anonymous]

did you ever figure out how to get the program to recognize the feed speeds? The post processor I down loaded does work fib=ne. Previously using MADCAM, Mach 3 Metric post processer worked fine.

[Anonymous]

very thank you. your post is working well. can you guide me where I can learn more about post process? what they contains and how I can change there code for my needs?

[rothmaind]

Works great, but converts everything to metric, and we have to scale everything up by 25.4 any way to to have it post out in imperial?

Thanks,

Daniel

[Anonymous]

I doubt it converts to metric, it is natively metric.

Isn't it probably time you learned metric like the other 95% of the world? 

[Anonymous]

Hi everyone,

I also have Weihong controller in my CNC router and I tried this post processor: "10717_Weihong NCstudio_with arcs.cps" but something's wrong. The machine works louder than normally when I use 2D CAD/CAM called Ucancam.

I think it's either wrong post processor or resolution of my machine (?) - maybe Fusion's tool path doesn't go with my machine.

Any ideas?

I recorded a short movie (with the spindle off) to hear better the machine moving along three axes.

I used 2D Adaptive Clearing. Smoothing: 0.01 mm.

I attach short movie clip and nc code.

Do you have any idea how to fix it?

Thanks,

Pawel

[Anonymous]

hello, i think problem is in smoothing, look at passes tab in toolpath menu, and look for enabled this option with a same number as a tolerance

maybe if you already enabled it, then problem may be in controller options

хотя, если по-русски читаете,мне будет проще объяснить)

[Anonymous]

Thank you. I think you're right. The same thing I heard from someone else yesterday. I used smoothing with default value of 0.01 mm which is probably too little and it makes the router to look for all these, close to each other, points on the tool path.

Do you recommend a better value for smoothing that won't cause this problem? I'll make some tests this weekend.

[Anonymous]

i think you should start a new topic with explanation your problem

mark me there

maybe it will interest someone else with a similiar problem

so my recommendation is something like this

if you input a stock to leave 0.5 mm so you may choose tolerance about 0.1 mm and smoothig 0.1 mm (there is something like a good rule choose smothing equal or greater than tolerance, but not smaller)

if you make no stock to leave then choose 0.01 tolerance and smoothing

it depends from what you need

i machining a steam turbine blade, so i need tolerances about 0.001 mm

but if you mill something like decorative vase you better choose tolerance like 0,05-0.1 mm for finish and about 0.5 mm for roughing(with about 1mm stock)

well, you still should look at controller preferences, maybe there is manufacturer options for smoothing, that conflict with your code

[Anonymous]

Thank you for your advice concerning proper smoothing values.

I'll also start a new topic about this issue.

Я еще не научились этому

[Anonymous]

I did not start a new topic.


The cause of the problem that I experienced was too tiny solid in which I tried to cut pocket. I did it only for testing, but it was too small, when I enlarged it, the problem disappeared.

This postprocessor works well with my CNC router.

[Anonymous]

My CNC router uses an NK105 G2 (not a G3). I downloaded the post you offered here and ended up with an error. It wouldn't process the path. Below is the error I'm getting. Is there anywhere to find a post to use with my model Weihong?

Error log:

Checksum of intermediate NC data: 43bdab6e8992f981d5359b225983ca16
Checksum of configuration: e1172929d066b15368ccc8164be0074d
Vendor url: http://www.autodesk.com
Legal: Copyright (C) 2012-2014 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.5331
...

###############################################################################
Error: Tool orientation is not supported.
Error at line: 378
Error in operation: 'Drill2'
Failed while processing onSection() for record 308.
###############################################################################

Error: Failed to invoke function 'onSection'.
Error: Failed to invoke 'onSection' in the post configuration.
Error: Failed to execute configuration.
Stop time: Tuesday, January 22, 2019 2:18:56 AM
Post processing failed.

[Anonymous]

hello

probably problem in axis of hole not alighned with z axis

check it

i think weihong uses g2 and g3 commands both

but you free to disable this function

[ArjanDijk]

Today I implemented a post for this machine. If anyone is concerned: I killed of all circular movements and replaced them by linear. Somehow the toollength (or just Z coordinates) were off by 8mm when using G2/G3. First I only killed G18/19 but later on also G17.  I did not notice a difference in how fluent it runs but the machine seemed like it had pretty agressive deceleration settings, so maybe just not so visible.

2 parts were screwed because it machined almost into the table

[FreezeS]

I am very interested in this. Is it published somewhere?

[Anonymous]

I'm not sure if that's what you mean, but here are two versions of manual and the post processor itself 🙂

https://www.weihong.com.cn/en/uploads/soft/160608/1-16060PUT0.pdf
https://am.co.za/router/panel/nk105.pdf

https://forums.autodesk.com/autodesk/attachments/autodesk/218/4961/1/10717_Weihong%20NCstudio_with%2...

[Anonymous]

Thanks a LOT! it worked 🙂 I am using NK105 G2

Autodesk should include it on their HSM and Fusion360 products as default since it is very common now days to use such a controller. 

Just two comments, on the post processor options use as follows:

1. Allow helical moves : NO

2. Use mm as unit. I noticed that if I have the file Units on inches, the cnc code will do smaller movements thinking you give it mm instead of inches. 

Best regards,