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

How to remove all unnecessary heights and clearances in Fusion 360?

Anonymous

How to remove all unnecessary heights and clearances in Fusion 360?

Anonymous
Not applicable

Hi, I am baffled by the quantity of heights and clearances in Fusion 360.

 

For example, for 2d contour I have:

Clearance height

Retract height

Feed height (true, this one can be disabled but you have to do it manually each time which is annoying)

Top height (ok this one is necessary but still it counts)

 

then you have under "Linking"

Safe distance

Lift height

and if you select "Ramp"

you have 

Ramp clearance height

 

Whats with all these heights and clearances? Why is it necessary? I don't see it as necessary, I see it as nuisance.

7 heights for just one thing?

 

This is what I need my G-code to look like:

G43 H2 Z5.

G01 Z0. F1000.

 

not like this:

G43 H2 Z15.5

G00 Z10.

G00 Z5.5

G00 Z2.

G1 Z0.

 

wtf?

 

 

Also, is there a way to create templates and defaults for tool links and compensation?

I need to have compensation always "In control" for mills (T2 and T3 mostly) and compensation "In computer" for T4 (chamfer mill).

I also always have to manually edit links to remove those stupid vertical and arc moves, I just need one thing active:

Linear lead in distance. Nothing else.

 

Thanks, any help is much appreciated.

0 Likes
Reply
1,276 Views
7 Replies
Replies (7)

seth.madore
Community Manager
Community Manager

I'm going to show you something that's going to totally blow your mind: Setting defaults.

Go into a toolpath.

Change everything to how you want it to be, reflective of your preferences and settings.

Click on any text box and select the "Make All Default" button:

2020-11-03_04h50_39.png

 

As for the Heights, here is my preferences, which will get you pretty close to what you are looking for:

2020-11-03_04h51_50.png

 

If at any point you decide one of the settings is not ideal, right click on the toolpath and select "Compare and Edit". Once in that new dialog, you can right click on almost any field and change the default behavior.


Seth Madore
Customer Advocacy Manager - Manufacturing
0 Likes

rhdfmail
Advocate
Advocate

Those in the heights-tab is for controlling the whole toolpath. Those under linking and  ramp-settings are for controlling specific parts of your toolpath.

You might want to have your retracts at 2mm above part, but you dont want your ramp or helix start up there and cutting air 

in pockets or in adaptive-ops you often want to keep the tool down as much as possible instead of lift to retract-plane between each move. Lift height prevents the tool from dragging across the surface

I Agree that  the extra rows in the G code can be annoying, but when running a program for the first time it can be used as a sanity-check :winking_face: Tool stops 10mm above stock instead of doing a rapid to -50...


You shoud be able to create a toolpath  with all the settings as you want them, rightclick on it and select "store
 as template" Save it as (as an example)  "2D-contour-T2"
Next time you want to use it, just rightclick on the setup and select "import from template".
Then edit the imported operation(s) and select geometry

You can also rightclick in most of the textfields and select "make default". In that way that value (or expression) will always be there for that type of operation. 

0 Likes

Anonymous
Not applicable

Okay that is something, but still I see no way to make defaults for each individual tool.

For example T2 is rough mill, it needs to have axial and radial material left after it mills part.

T3 is for finishing, flat end mill, it doesnt need axial and radial material left after it mills part.

T4 is chamfer mill, it doesnt need compensation so it needs to be "In computer" instead of "in control".

 

All of those things aren't saved for each tool using your method.

I still need to change every tool in new part after everything was saved in last part. No defaults for each tool.

 

Also, I want universal tool library, I don't want my changes keep effect in next part beacuse what I change in my tool library for last part, will stay saved for next part.

How to have universal tool library so every tool saved there stays the same for each and every new part I am creating?

 

Why is "Stock box point" default while choosing WCS and not "Model box point"? Why is "model orientation" default and not "Choose Z plane and X axis"?

Final question, why if I use "in control" for chamfer mill and leave all settings the same as in "in computer" my chamfer mill will creata alot bigger chamfer than necessary, like it alters path for that tool with changing from "in computer" to "in control"?

0 Likes

seth.madore
Community Manager
Community Manager

There's a LOT of stuff packed into your last question. I'll address most of them here, as I can.

1) Defaults for each tool; for some toolpath settings, this is not possible. You can set stepover/down at the tool level via Presets (using the new Tool Library) Is T2 ALWAYS roughing, same size tool? T3 is ALWAYS finishing, same size tool as always?

If so, create Templates. Program a generic part, setting all your toolpaths to your preferences. Select all your toolpaths, right click and "Store as Template"

2020-11-03_09h21_01.png

 

Stock Box and Model Orientation are defaults. Those too can be changed. Change them to your preference and right click in a text box (program comment, for example) and select "Make All Default"

 

Unsure what you mean about Chamfer and compensation. Can you share an example?

 


Seth Madore
Customer Advocacy Manager - Manufacturing
0 Likes

Anonymous
Not applicable

Okay, thanks again for the info.

 

I also wonder why there needs to be a lead in and lead out when using "In control" compensation type?

There really is no need for this, in SolidCAM, you can select none and it will still generate your G-code, there only needs to be Radius of tool value for space in order to build compensation. Why is it not like this in Fusion?

 

I have a problem while creating small slot 3mm wide with 2mm end mill. I need to have compensation "In control" and ramp moves (spiral/helix toolpath) at the same time, but I had big problems with that and couldnt do it ultimately.

 

I had to change tolerance value under Passes tab to 0.4 (or 0.5mm, not sure anymore) and I've put 0.13mm lead in lead out (straight line) but still my 2 mm end mill crashed into slot contour every time, even though 0.5mm space on each side around the mill in that slot is more than enough for it to build compensation and not crash into slot contour.

 

This was done under 2d Contour operation, I've tried many others, both 2d and 3d operations and couldn't have both compensation turned on (In control setting) and ramp/helical toolpath for the mill.

 

What is the problem with this?

0 Likes

SendItCNC
Advocate
Advocate

Hey Seth, 

 

Just curious on your preferred Clearance Height being Model Top + 0.1. Seems to invite collisions when Stock Top is more than 0.1 above the model top. Of course those can be sorted out in simulation, but curious about the thinking behind that choice.

 

Looks like the built-in defaults are set very conservatively, which is understandable.

 

Useful tip on setting defaults in Setup, thanks!

0 Likes

rhdfmail
Advocate
Advocate

Normaly there will just be stock material on top of the part for the first one or two ops.

Instead of having to change heightsettings for all ops you only have to change them for those where you might crash into stock

If you want a universal template with some security and just import and run the code, you might want to have the clearence-plane above the stock.

0 Likes