Warning: Tool number exceeds maximum value.

[AdCNC]

Hi There,

Can anyone help me out as I'm having trouble in getting HSMxpress to post with high tool numbers.

All my chamfer tools start at 600, can anyone tell me what i have to do to the post to get around this error

Warning: Tool number exceeds maximum value.
Error: Length offset out of range.
Error: Failed to invoke function 'onSection'.
Error: Failed to invoke 'onSection' in the post configuration.
Error: Failed to execute configuration.

As soon as i lower the number to say 200 its fine.

Machine is a Hurco VM20 2012 running winmax 7

OR if anyone has a post the would like to share that could rectify this problem that would be much appreciated

Cheers

Ad

[George-Roberts]

Could you upload the post you are using? It would be an easy modification to sort this out

[AdCNC]

Hi George, im using the stock hurco.cps

Please see attached file.

Regards

Ad

[skidsolo]

the tool length offset number of for the machine is limited by this line of code:

      if (lengthOffset > 200) {
        error(localize("Length offset out of range."));
        return;
      }

This may be a limit for the machine contoller, can you tell us the maximum tool offset number that the controller can address ?

[AdCNC]

Hi The control can accept up to a 5 figure number theoretical 99999

[AdCNC]

Ive just modded the post to 

if (lengthOffset > 99999) {
        error(localize("Length offset out of range."));
        return;
      }

and all seems to be well so far.

[Anonymous]

I'm having the same exact problem with my software except it's capped at 99 tools. I'm wondering where the code below exists for me to edit? I'm using a Mac by the way.

if (lengthOffset > 99) {
        error(localize("Length offset out of range."));
        return;
      }

Thanks!

MB

[George-Roberts]

You will need to modify the post processor. If you edit the post you are using and just use the find command in a text editor, you should find the value you are after 🙂 what post are you using?

[Anonymous]

Ok...Assume I know nothing. Ha. When you say post do you mean post processor? If so, I'm just using whatever it is fusion offers inside the program. I'm pretty new with this software and cam software in general by the way. Sorry, I don't know what you mean by opening the post in a text editor. Obvs I know what a text editor is=) but the rest is sort of confusing to me. Can you explain in some more detail?

Thanks!

-MB

[George-Roberts]

I apologies for my last vague response, I was replying off my phone. Luckily I'm at my computer now so can give a more detailed response.

First, setup some toolpaths in Fusion 360 and click 'Post Process' on the ribbon bar

This will open a dialog where you can select the post processor for your machine. Select the correct post processor and choose 'Open config':

This will open the post up in a text editor (probably brackets). If it doesn't, open the post from the folder location shown under the 'Configuration Folder' section in the post processor window. Use the text editor find function (CMD + F) to find the following lines:

•  if (tool.number > 99) {
•  if (lengthOffset > 99) {
•  if (d > 99) {

Then simply change the 99 value to whatever you want the highest tool number to be (maybe 99999 or something). Make sure you keep all the brackets and formatting the same. Just change the number

Finally, save the post in a location where it will not be overwritten. In the Fusion post processor window, you will need to navigate to the location you stored the post by clicking the three dots here:

Hope this helps 🙂

[Anonymous]

No worries! That helps a lot yes I now understand exactly what you are doing. Unfortunately, I think we're using different operating systems. I'm on a Mac and it doesn't have any of those extra options to open a config file or view the path of the config folder. Unless I'm totally missing something which is always possible=). I really appreciate your help!

-MB

[marcusjung]

Boa noite.

Alguém poderia me ajudar com esses dois avisos? Alguém já passou por isso?

[Andy_Phillips]

Hello - I have been using F360 and the Fusion360-supplied post processor for my Nomad for several years.  Today I started to get the message that the tool number exceeds 100 maximum error.  This is tricky as the Carbide3d tool library has tool numbers from 100 upwards (e.g. 101 and 102).  I see that the post-processor changed on March 13 2023.  I downloaded the previous post-processor and it works without issue so I assume we have an issue with the recent release.  Can somebody correct the post processor for Carbide3d?  Thank you.

[AchimN]

Hello @Andy_Phillips ,

thanks for your feedback.

Yes there was indeed a change on that with the last post update. You should get a warning but not an error, is that correct?

When the control does allow tool numbers above 100, you can add that to the settings object at the top of the postprocessor with this:

maximumToolNumber : 9999 // specifies the maximum allowed tool number

or in case you are using a machine configuration, you can change the maximum number of tools to your desired value.

Hope this helps!