Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Engraving gcode error - entry and exit marks

11 REPLIES 11
Reply
Message 1 of 12
Natalie_CKD
219 Views, 11 Replies

Engraving gcode error - entry and exit marks

Hi,

 

I just started to use fusion for plastic engraving with a CNC. The gcode exported from fusion has these entry/exit lines that drags along the plastic which isn’t found in the fusion drawing. Any ideas what I’m doing wrongly? 

11 REPLIES 11
Message 2 of 12
HughesTooling
in reply to: Natalie_CKD

Really need more info, can you share the f3d file?

One thought is have you got keep tool down checked? Try unchecking it.

HughesTooling_0-1708511025272.png

 

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 3 of 12
seth.madore
in reply to: Natalie_CKD

Do you have your heights set correctly at the machine?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 4 of 12
Natalie_CKD
in reply to: Natalie_CKD

Hi @HughesTooling 
Checking my setups, the "keep tool down" is unchecked.

CKDsb_0-1708526706155.png

 

 

 

I created another file with a simple box and circle, and its still showing these "unwanted" engraved lines. When simulating on Autodesk Fusion the path seems correct, however upon exporting .tap to Mach3, the g-code shows this on Mach3 screen:

 

CKDsb_2-1708527180916.png

 

CKDsb_1-1708527114755.png

 

Attaching files here for reference.

 

 

Message 5 of 12
Natalie_CKD
in reply to: Natalie_CKD

Hi @seth.madore 

 

The heights for the engraving text & lines are correct and reflected correctly when engraving. I cant figure out why the gcode exported from Fusion360 adds this additional "unwanted lines'. I had a friend create a similar design on ArtCam and exported to gcode. I then used this file to upload to my Mach3 and it doesn't have this issue.

 

Thanks!

Message 6 of 12
seth.madore
in reply to: Natalie_CKD

@Natalie_CKD what post processor are you using, can you share the code that you were getting?

 

I just posted this out with the Mach3 post processor, and this is what I'm getting:

2024-02-21_10h08_10.png


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 12
Natalie_CKD
in reply to: Natalie_CKD

Hi @seth.madore  


Attaching the g-code exported as .tap from Fusion360 - uploading the .txt file here (unable to upload .tap to this thread).

 

I'm using Mach3mill. May I ask what Mach3 post processor application you are using? 


Message 8 of 12
seth.madore
in reply to: Natalie_CKD

It's not a Mach3 screen that I shared with you, it's what is referred to as a "backplotter" (I use Cimco Edit).

Now, can you share the code that your friend gave you? (your code looks the same as what I showed earlier, and is correct, by all accounts)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 12
HughesTooling
in reply to: seth.madore

Is this the old G28 problem on a machine that hasn't been homed?

HughesTooling_0-1708532374656.png

@Natalie_CKD There are options on the post dialog for different retracts but I'd recommend setting your machine home position and using G28. Some info on G28.

 

 

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 10 of 12
seth.madore
in reply to: HughesTooling


@HughesTooling wrote:

Is this the old G28 problem on a machine that hasn't been homed?

 


It does sound like it


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 12
Natalie_CKD
in reply to: Natalie_CKD

Hi @seth.madore  and @HughesTooling 
 
Finally received a reply from my CNC machine seller. He stated that the CNC machine supplied is to be used with Mach3 Mill + ArtCam thus he is not supporting my inquiries for Fusion360 + Mach3 Mill.

 

I tried using Artcam and it does not have the same issue as what I'm facing with described above in Fusion360. There must be some machine settings / home settings that I'm missing out? 

 

 

Message 12 of 12
HughesTooling
in reply to: Natalie_CKD


@Natalie_CKD wrote:

 

I tried using Artcam and it does not have the same issue as what I'm facing with described above in Fusion360. There must be some machine settings / home settings that I'm missing out? 

 

 


A lot of the cheaper CAM systems do not use G28 for tool changes, bit amateurish really!

 

The problem you're reporting comes up all the time and is because you're not setting the machine home position. Usually you would have limit switches and home the machine but most of the Chinese machines don't bother. If you do some research you can find out how the set your machine home position(G53). You should then set you job using G54 as your origin.

 

If you want to just bodge it you also have the option to do it the same way as ArtCAM.

On the post dialog there's an option for safe retracts, you can select clearance height but be careful as you can run into problems with tool changes and also run the risk of running the machine into the mechanical limits. Personally I'd recommend buying and fitting limit switches and doing it the right way.

HughesTooling_0-1709023189231.png

 

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report