Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.
Anonymous
599 Views, 15 Replies

2DAdaptive Refuses to Remove All Material

In the attached model, I have been completely unable to get the "Perimeter Roughing" operation in the second setup to remove material from all four sides of the model.  It does three sides, and stops short of doing the fourth, even if I put a ton of extra stock out there.  Why??

 

Regards,

Ray L.

ivan.stanojevic
in reply to: Anonymous

Your model does not contain any operations. 

Could you upload it again? It will be easier to check where is the issue coming from if we can see your programming workflow.

 



Ivan Stanojevic


Anonymous
in reply to: ivan.stanojevic

OK....  I did an Export.  How do I make it include the CAM stuff??

 

Regards,

Ray L.

Anonymous
in reply to: Anonymous

Try This one...

Anonymous
in reply to: Anonymous

BTW - In the same model, the threadmill operation fails in POST.  I'd REALLY like to know what's going on there, but it tells me to look at the "log file" but gives no clue where the log file is!

 

Regards,

Ray L.

Steinwerks
in reply to: Anonymous

With regard to your threadmill operation being bonkers, it has something to do with Hole Top and Hole Bottom. If you manually select the top and bottom edges of the hole, the top and bottom heights are displayed although they were not before.

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Anonymous
in reply to: Steinwerks

OK, but it still fails in POST even when I select faces for Top and Bottom.  And Hole Top and Hole Bottom SHOULD work here, exactly like they do for drilling operations (and like they do in HSMXpress).

 

Regards,

Ray L.

Steinwerks
in reply to: Anonymous

Alright, with 2D Adaptive you have a LOT of things selected for this chain and that's the issue, it's sort of colliding with itself.

 

I X'd the old selection and selected the following outside portion of the chain:

 

Selection 1.jpg

 

 

Then I clicked the red arrow to reverse the direction (really wanted to cut inside the chain) and turned on Stock Contours:

 

Selection 2.jpgSelection 3.jpg

 

Edit: I'll add that your Perimeter Finishing toolpath has the same issue. Reselecting the chain as I did in 2D Adaptive cut the toolpath from 22.6k to 4.7k.

 

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Steinwerks
in reply to: Anonymous


@Anonymous wrote:

OK, but it still fails in POST even when I select faces for Top and Bottom.  And Hole Top and Hole Bottom SHOULD work here, exactly like they do for drilling operations (and like they do in HSMXpress).

 

Regards,

Ray L.


Yes I understand there's an issue going on, but it turns out it's likely a tool number issue. What post processor are you using? This was the stock 3-axis Haas post.

 

Information: Configuration: Generic HAAS
Information: Vendor: Haas Automation
Information: Posting intermediate data to 'C:\Users\***\Desktop\10.nc'
Information: Total number of warnings: 2
Error: Failed to post process. See below for details.
...
Code page changed to '1252  (ANSI - Latin I)'
Start time: Saturday, April 22, 2017 2:00:57 AM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 41304
Configuration path: C:\Users\***\AppData\Local\Autodesk\webdeploy\production\ba8d00e1d3edcf8bc857786ba8a2c11fa2b8c071\Applications\CAM360\Data\Posts\haas.cps
Include paths: C:\Users\***\AppData\Local\Autodesk\webdeploy\production\ba8d00e1d3edcf8bc857786ba8a2c11fa2b8c071\Applications\CAM360\Data\Posts
Configuration modification date: Wednesday, March 1, 2017 10:30:22 PM
Output path: C:\Users\***\Desktop\10.nc
Checksum of intermediate NC data: dba18e940ac3fae00eb8ae26e12ea572
Checksum of configuration: 1b08930933be113d79adec9f2ab4c53f
Vendor url: https://www.haascnc.com
Legal: Copyright (C) 2012-2017 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.2989
...
Warning: Tool number exceeds maximum value.
Warning: Work offset has not been specified. Using G54 as WCS.
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.
Stop time: Saturday, April 22, 2017 2:00:57 AM
Post processing failed.

 Edit: is this the same post you've been using for HSMXpress?

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Anonymous
in reply to: Steinwerks

I'm using a custom POST that I've been using for years with HSMXpress.  If it's a POST issue, I'm happy to debug it, but I have yet to find the log file that tells me what/where the problem is.  I have another thread asking where that log file goes.  In HSMXpress, it get written to the .c file in place of the G-code, but Fusion just puts a message in the g-code telling me to look at the log file, but doesn't give me any clue WHERE that log file is written to!

 

Regards,

Ray L.

Steinwerks
in reply to: Anonymous

Can you share the .cps file here? I don't really want to edit a post just to get past the tool number issue to find out what the REAL issue is. If you don't want to share it publicly you can email it to me at steinwerks at gmail dot com.

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Anonymous
in reply to: Steinwerks

OK, so selecting JUST the solid-lined profile in the sketch solves the problem.  But there is no visual indication of any problem when the entire sketch is selected - it displays the CORRECT profile in blue.  So, how would I have known it was unhappy?  In Solidworks/HSMXpress, construction lines are completely ignored by CAM, only actual drawing lines are "seen" as profile selections.  That would be a really nice change to make in Fusion.

 

Regards,

Ray L.

Anonymous
in reply to: Anonymous

One more comment:  "Pocket Selections" in the that dialog is really mis-leading.  It's not necessarily a pocket, as in my example.  It should be "Profile Selections" or something similar.

 

Regards,

Ray L.

Anonymous
in reply to: Steinwerks

.cps file attached.

 

Regards,

Ray L.

Steinwerks
in reply to: Anonymous

Construction lines in HSMWorks are certainly not ignored entirely, but only when you select an entire sketch. You can select them manually.

 

 

At any rate, this is not SolidWorks and can't always be expected to behave exactly the same. The underlying CAD is completely different. I certainly agree that CAM ignoring construction lines is a a great idea and I support adding it to the Ideastation here: https://forums.autodesk.com/t5/hsm-ideas/idb-p/231

 

I'll see what I can dig up with your post now.

 

And yes, Pocket Selection has been argued as poor wording already but it got us nowhere. 

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Steinwerks
in reply to: Steinwerks

Your post isn't set up for the threadmill and fails: "Error: UNKNOWN CUTVIEWER TOOL TYPE: 38"

 

Your .log files should be located here (possibly in a subfolder, this one was in '3'): C:\Users\*username*\AppData\Local\Temp\Fusion360CAM

 

I suspect that the file open command isn't getting to Brackets fast enough. If you can change the editor to the HSMEditor.exe, I would suggest it. It's much better at catching those commands and launching in time.

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube