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: 

Stock Collision Issues

16 REPLIES 16
SOLVED
Reply
Message 1 of 17
jerome
1087 Views, 16 Replies

Stock Collision Issues

I'm using 3d parallel in CAM fusion 360 and I have an issue about toolpath bit travel form start poiint(Zero) and where the bit is supposed to enter in the stock. For now, it's going straight into the stock to the entry point and do not travel above stock material to the entry point.
When the job is done the bit travel straight accros the model to the start point.
Any idea about my problem? Which parameter should I change in the 3D parallel tool to travel above the stock? I increased Retract Height and Clearance Height but it changed nothing.


Thanks.

16 REPLIES 16
Message 2 of 17
ivan.stanojevic
in reply to: jerome

Hi,
3D parallel strategy is intended for finishing only and it will generate the toolpath only on surface of the model and that is the reason why it crashes with your stock. However, you can add axial offset passes if you want to do the roughing with 3d parallel. If you share/attach your model or a screenshot, I could take a better look to see what is going on.


Ivan Stanojevic


Message 3 of 17
Steinwerks
in reply to: jerome

I believe this is a home position issue. What is the machine and control @jerome ? Have you set up a machine home position or do you home it using the tool on top of the stock?
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
Message 4 of 17
jerome
in reply to: ivan.stanojevic

Hi Ivan,

 

As you can see on the pictures, I set the zero point on the upper left corner. The others pictures are the 3d parallel path settings.Setup-Stock-Box.png

3d-Parallel-0,25.png3d-Parallel-0,25-Clearance.png3d-Parallel-0,25-Geometry.png3d-Parallel-0,25-Linking.png3d-Parallel-0,25-Passes.png

I know it's a finishing tool, but my biggest problem is whene the job is done, the toolpath is going straight in the model and cut it all the way to go back at the starting point.

 

Thanks,

Jerome

Message 5 of 17
jerome
in reply to: Steinwerks

Hi Neal,

 

The home position is like all of the previous home I did in my past projects.

It's going straight at the starting point at the right corner of the model. When the path is finished, the bit is going straight at the starting point across the model.

I don't thing it's CNC related because it's doing that in the toolpath simulation.

I use an X-Carve 1000mm.

Setup-Stock-Box.png

 

Thanks,

Jerome

 

Message 6 of 17
ivan.stanojevic
in reply to: jerome

Did you select your model in the setup?

 

2017-03-20_1323.png

 

It's really hard to say without looking at the part.



Ivan Stanojevic


Message 7 of 17
jerome
in reply to: ivan.stanojevic

Yes I selected my model.

Here is a link to my model you should see what happen?

http://a360.co/2mHVzct

 

Thanks

 

 

Message 8 of 17
ivan.stanojevic
in reply to: jerome

Hi Jerome,

Could you please explain what are you trying to achieve?
By looking at your part I don't see that anything is wrong except that you don't have any roughing strategy to machine the outer material.
3D parallel toolpath is doing exactly what I told you in the previous post.

 

Just to be clear, as a finishing strategy 3d parallel is not going to machine your stock, it will machine only model surfaces.



Ivan Stanojevic


Message 9 of 17
jerome
in reply to: ivan.stanojevic

Hi Ivan,

I can live with the starting sequence, but my biggest problem is when it's finishing the path. At the end, the tool is back at the starting point and it pass accross the model as you can see on the picture.

20170320_130407.jpg

 

Thanks,

Jerome

 

Message 10 of 17
Steinwerks
in reply to: jerome

I'm guessing the end of the program features a G91 G28 Z0. which puts the tool right back to the top of the stock. Then it goes to X0 Y0?

 

Edit: @jerome can you share which post processor you're using (or attach it here)?

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
Message 11 of 17
ivan.stanojevic
in reply to: jerome

Hi Jerome,
I see now, sorry for misunderstanding, but I can tell you that you did nothing wrong in the Fusion.

@Steinwerks could you please take a look at this? I think that you were right.



Ivan Stanojevic


Message 12 of 17
jerome
in reply to: ivan.stanojevic

Thanks, Ivan,

 

As you said Steinwerks, the end of the file is

M9
G28 G91 Z0
G28 X0 Y0
M30
%

 

If I understand correctly, the Z should not be zero but the original starting point "Z15.747".

Am I wrong?

 

Thanks,

Jerome

Message 13 of 17
Steinwerks
in reply to: jerome

@jerome

 

That line is a home position move meant to move the machine to its maximum travel limit. Many small hobby-size machines do not have limit switches and most of the CAM softwares that come with them never try to move the machine to home position after the program runs. The CAM in Fusion was developed around industrial work and ALL machines that I have ever seen have home positions from which all work coordinates are derived and so this is a known position to the machine and usually very far from the workpiece.

 

Which post processor are you using? Some of them include options in the dialogue to turn off home positioning, at which point the machine will retract to the Clearance Height and stop (or possibly go to the home position).

 

UseG28.JPG

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
Message 14 of 17
jerome
in reply to: Steinwerks

I use Generic GRBL postprocess.

Message 15 of 17
jerome
in reply to: jerome

G28 parameter is setted at YES.

Message 16 of 17
Steinwerks
in reply to: jerome


@jerome wrote:

G28 parameter is setted at YES.


Set it to NO when you post your program and run carefully.

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
Message 17 of 17
jerome
in reply to: Steinwerks

Thank you very much.

 

Jerome

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

Post to forums  

Autodesk Design & Make Report