- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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![]()
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
OK.... I did an Export. How do I make it include the CAM stuff??
Regards,
Ray L.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.
Find me on:
Instagram and YouTube
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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:
Then I clicked the red arrow to reverse the direction (really wanted to cut inside the chain) and turned on Stock Contours:
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.
New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.
Find me on:
Instagram and YouTube
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
@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?
New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.
Find me on:
Instagram and YouTube
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.
Find me on:
Instagram and YouTube
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.
Find me on:
Instagram and YouTube
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
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.
New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.
Find me on:
Instagram and YouTube
Fusion