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: 

PostProces CHANGE Cutting Feedrate WARNING

14 REPLIES 14
Reply
Message 1 of 15
veso58S5W
585 Views, 14 Replies

PostProces CHANGE Cutting Feedrate WARNING

WARNING   WARNING   WARNING
After latest update, PostProcess change Cutting Feedrate on it's own to the same as Ramp or Plunge Feedrate (default 333.333mm/min)
Who knows what else is wrong in Manufacture? Toolpath? Cuts? Speed?

Here is a photo of my Cutting Feedrate.

Attached is the NC Code file.

Open it to see line N95. F333.3 is totally wrong!!!!!!!!!!!!!!!!!!!!!!!

Feedrate.jpg
WARNING   WARNING   WARNING
AutoDesk:
Immediately fix problems with Manufacture in Fusion360.
You might be liable for huge damages in material, injuries and human life.

14 REPLIES 14
Message 2 of 15
HughesTooling
in reply to: veso58S5W

I'm not seeing the problem in my test file. Going to need more info. Can you share your design or mock something up to demonstrate the problem also what postprocessor are you using?

 

Thanks Mark

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 15
veso58S5W
in reply to: HughesTooling

1. I don't know what you mean saying - "test file"?
2. Design doesn't have nothing to do with CAM part of the program. It is a simple box what I want to cut with 2D Contour.

3. I use what Fusion supplied for Fadal CNC. Here is a photo attached.

You can see that it was updated on 3rd. EXACTLY after that update I got problems.

This is not the only one. Fusion behaves like retard now.

This is really horribly dangerous.

Post switch feed rates, thus run machine very slow in Cutting Feed.

Such things can have severe consequences.

Post.jpg

Message 4 of 15
veso58S5W
in reply to: HughesTooling

I just played with 2D Contour settings, and tested toolpath editing box/F360 Postprocess.

What is happening is this:

Fusion Postproces takes Ramp Feedrate and throw it instead Cutting Feedrate (after G1..... command) what was set in editing box of the toolpath.

THAT IS HORRIBLE MISTAKE

Message 5 of 15
daniel_lyall
in reply to: veso58S5W

In the Gcode you supplied there is 6 333.3 moves and it is the plunge feed rate doing it,  you only plunge into an existing hole otherwise it can and will break a cutter a user risk.

All this is simple to test for set the plunge rate to a stupid amount.


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

Message 6 of 15
veso58S5W
in reply to: daniel_lyall

Please DO NOT REPLY to messages without any meaning to the problem.

You didn't supply any solution.

Message 7 of 15
HughesTooling
in reply to: veso58S5W


@veso58S5W wrote:

1. I don't know what you mean saying - "test file"?
2. Design doesn't have nothing to do with CAM part of the program. It is a simple box what I want to cut with 2D Contour.

 


By "test file" I mean I made a file to test because you can't be bothered to supply a design that shows the problem. So I made another test file that looks somewhat like yours and posted with the Fadel post and it works fine so unless you can be bothered to supply a file I doubt anyone can help.

Here a back plot, ramps are dark brown(500mm/min) and cutting feed rate are green(2500mm/min). Shows the feed is changing between all ramps and levels.

Old.png

Mark

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 8 of 15
HughesTooling
in reply to: veso58S5W

Ok just backplotted your file from the first post and don't see what's wrong.  Plunge is at 333, lead in 1000 then ramp 333 when it reaches depth feed changes to 2558, changes to 639.5 for corners does this every level?

image.png

Mark

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 9 of 15
veso58S5W
in reply to: HughesTooling

Did you run this script on CNC? Probably didn't. Othervise you'll see that your Cutting FeedRate is 333.333.
I don't know your experience, I don't know who you are. But, what you made here shows that I am right.
F360 takes value of Plunge FeedRate and place it in/as Cutting FeedRate. Somebody made horrible mistake in that update.
If you have contact with them, PLEASE warn them.
I red on other forums people already crashed their machines. 

Message 10 of 15
HughesTooling
in reply to: veso58S5W


@veso58S5W wrote:

Did you run this script on CNC? Probably didn't. Othervise you'll see that your Cutting FeedRate is 333.333.
I don't know your experience, I don't know who you are. But, what you made here shows that I am right.
F360 takes value of Plunge FeedRate and place it in/as Cutting FeedRate. Somebody made horrible mistake in that update.
If you have contact with them, PLEASE warn them.
I red on other forums people already crashed their machines. 


 

No I didn't run it on the machine but the G code is correct if you can't see that you don't have much experience yourself. The code you posted shows the ramps are cut at 333 and all toolpaths at each level are cut at 2588. You can see in your code the first 333.33 feed is on the plunge then it changes to 1000.00 for the in feed then back to 333.33 for the ramp, the next 6 lines are all ramp moves with the Z moving then when it reaches 10mm depth it changes to 2558mm this is all correct, if your machine is doing something different it's not down to Fusion or the G code.

If your machine is doing something different it's a problem with the machine not the G code. Perhaps you should contact the machine supplier.

 

Mark

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 11 of 15
HughesTooling
in reply to: veso58S5W


@veso58S5W wrote:


I don't know your experience, I don't know who you are. But, what you made here shows that I am right.


As you asked about my experience, I started using computers in 1982, started with CAD in 1992 and CNC in 1996. I use Fusion every day to program 6 mills with 4 different controls, 2 lathes and 2 4 axis wire eroders so yes I can read G code and no what I've posted and what you've posted shows there's no problem with the code. If your machine is not doing what the code requests the problem's with your machine.

 

This is from your file. This is all correct and giving the feed rates you've set.

N60 G43 Z40. H2
N65 Z15.
N70 G1 Z11. F333.3                      <--------------------Plunge feed rate
N75 Z2.973
N80 G19 G2 Y166.811 Z0.5 J-2.473
N85 G1 Y164.338 F1000.                  <--------------------Lead in feed rate
N90 G17 G3 X433. Y161.865 I2.473
N95 G1 X874.865 Z-0.962 F333.3          <--------------------Ramp feed rate
N100 Y-11.865 Z-1.538                   <--------------------Ramp feed rate
N105 X-8.865 Z-4.462                    <--------------------Ramp feed rate
N110 Y161.865 Z-5.038                   <--------------------Ramp feed rate
N115 X874.865 Z-7.962                   <--------------------Ramp feed rate
N120 Y-11.865 Z-8.538                   <--------------------Ramp feed rate
N125 X433. Z-10.                        <--------------------Ramp feed rate. First level reached
N130 X3.5 F2558.                        <--------------------Cut feed rate
N135 X-3.919
N140 X-8.865 F639.5                     <--------------------Feed optimisation feed rate
N145 Y156.919 F2558.                    <--------------------Cut feed rate
N150 Y161.865 F639.5
N155 X869.919 F2558.
N160 X874.865 F639.5
N165 Y0.5 F2558.
N170 Y-6.919
N175 Y-11.865 F639.5
N180 X433. F2558.
N185 X-8.865 Z-11.462 F333.3            <--------------------Ramp feed rate. Next level back to ramp feed

Mark

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 12 of 15
seth.madore
in reply to: HughesTooling

Sheesh! I take my daughters camping and the whole place falls apart!

@veso58S5W  I am not seeing this issue in my posted code. Please attach the Fusion file that you use to produce this error. Yes, it matters, as it contains all your CAM settings, and that is what will lead us to the most correct answer.

 

File > Export > Save to local folder. Return to thread and attach the .f3d file in your reply


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 13 of 15
HughesTooling
in reply to: veso58S5W


@veso58S5W wrote:

Open it to see line N95. F333.3 is totally wrong!!!!!!!!!!!!!!!!!!!!!!!

Feedrate.jpg

@seth.madore  Initially I didn't read the first post carefully as I wanted to see the f3d first. Now I see the OP says line 95 changes to a feed rate of 333.33 and it's the wrong feed rate. Trouble is the screengrab shows the ramp feed rate at 333.333 and line 95 is the first line of the ramp so it's correct. So no real need to see the file as the code is posting correctly.

 

Mark

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 14 of 15
adamNT4S4
in reply to: HughesTooling

At least, the your post processor isn't taking your feed rates and dividing it by 47.904 for all of your feeds. This is what I have set for my feed rates in fusion. Looks like someone pissed off your computer programmer before this last update. I had to manually change the feed rates in the gcode. It was melting the $375 sheet of HDPE that I was cutting destroying the sheet.

T6 Bit.JPG

Feed Rate.JPG

Message 15 of 15

this thread is over 4 years old.

My guess is you have something going on inside your Post (which you included no information about).

Please click "Accept Solution" if what I wrote solved your issue!

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

Post to forums