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.
Solved! Go to Solution.
Solved by Steinwerks. Go to Solution.
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.
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
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.
Thanks,
Jerome
Did you select your model in the setup?
It's really hard to say without looking at the part.
Ivan Stanojevic
Yes I selected my model.
Here is a link to my model you should see what happen?
Thanks
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
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.
Thanks,
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)?
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
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
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).
@jerome wrote:
G28 parameter is setted at YES.
Set it to NO when you post your program and run carefully.