Obviously this is also a Fusion forum question as well but wanted to get input here first. I want to start taking advantage of setting up probing when programming, it gets old manually probing and I have a long term product I want to maximize efficiency in my setup.
Anyone doing this? Can you shead some light on how I get started and any input on your experiences. I’ve played with it in fusion but have not ran it at the machine. What’s the workflow? What to expect at the machine?
Thanks
Bill, @David_Loomes has some excellent videos on this topic. Here’s one link , but there are others on his channel. I’m also starting to try to figure this out, so I’ll be watching this thread.
Bill
What you’re looking to do is called in-process probing. I use this type of automated probing in all my cam programs
It might take a few days, because I have a big non shop related project I’m in the middle of, but I will post a lengthy response for you by this weekend
Ed
Bill’
Sorry it took so long to get back to you
Let me start be describing my setup
I have a 3 year old 1100mx - I use 2 Tegara 660U vises
I have only used the Hallmark ITTP Probe
I make 18 different size parts with dozens of variations for each part
size ranges from 3"x3" up to 10"x14" - 3/4 to 1" 6061 plate
For each part there are 5 or 6 operations per part with removal from the vise each time
I use one or both vises at a time depending on orders
so I have hundreds of fusion drawings with 2-5 separate posts per drawing
The first operation for any part is initial surfacing - which the only critical probe is Z
I have a probing routine that I run first thing every morning that probes the outside edge and face of each fixed Jaw for X & Y and probes a dummy piece of stock mounted in each vise for Z
once I’ve done that I can surface any size part with no additional probing
I just load the appropriate file - align the stock with the fixed jaw and go (WCS is top Left or Right corner of raw Stock depending on which vise)
After surfacing the part is remove for polishing before the next OP
With the part back in the vise I now probe the part on all for sides and top making the WCS the middle of the part with Z being the machined and polished surface - all features are then machined on this side. having the WCS in the middle of the part means more accurate probing in my opinion.
I use a different WCS name for each size part and each operation for that part
so for each of the 18 different sizes I use 6 separate WCS’s that never change
I use what fusion call “extra” wcs’s in the setup - starting with G54.1P10
I only use the common G54 G55 etc. for one off stuff
Then part comes in and out several times to machine other features on different sides
with a probing routine each time
OK - after all that lets looks at how to setup in-process probing
Create a new setup for probing - lets say the WCS is in the center of a piece of rectangular stock
I always probe Z first - which is important
In the new setup select “Probe WCS” from the Setup tab in Fusion
The Tool Tab
Select your probe
Link Feedrate is fine at 120ipm
Lead-in Feedrate for probing Z is fine with the default 40ipm
Measure Feedrate of 4ipm also fine
Nothing to set in multi-axis tab
Geometry Tab
Select Stock or Model
Click the Z face - Initially it will display X-Y probing - just select "Z Surface" in the Probe Type drop-down
Generally the default Approach and Over travel won't need to be changed when probing Z
Also have never messed with Feature Tolerance
Heights Tab
Bottom Height should be "Probing Top Surface" - with no offset
Actions Tab - discuss this later
OK so now the Z height is set for your selected WCS - lets do X&Y
I’ll just discuss the differences
Tool Tab - I use 200ipm for Lead-In feedrate
Geometry Tab - Select the X&Y surfaces
Heights Tab - The Offset needs to be Negative - as a standard I use “-0.15” - this depends on your probe tip diameter - you don’t want to probe a burr protruding from the top
Basically that’s it - as with any new WCS you will have to manually probe the first time so your machine knows the approximate position of the WCS - each time you probe a new part the WCS changes slightly depending on part position in the vise - that’s why we are probing !
Detail on some aspects
I up the Link Feedrate when doing X & Y so it doesn’t take so long to get from left right or front back
Some times when probing for the center I want a different probe height on X vs Y to avoid a feature - I do this by separating the X and Y probing into different operations and changing the Bottom Height longer on one or the other
Approach in Geometry Tab - this is the distance that the probe starts its cycle away from where it expects to find the surface - generally the default is fine - if you are probing a bore you will have to reduce this number to fit the bore
Over Travel is the distance the probe will move AFTER the point where it expects to find the surface being probed
If you want you can set your WCS at the center of a bore and probe the bore in-process
Same for a Boss or a slot
The Action Tab
This tab has advanced options - personally I have not used any of them
Override Driving WCS - is something I still try to wrap my head around how its useful - there are very few videos on the subject.
Wrong Size uses the Feature Tolerances from the Geometry tab to through a warning if you stock is out of the specification.
Give it a try and see how you like it
If you have any questions I will try to answer them
Ed
I just recently looked into this as I’ve been using the excellent post processor from David Loomes.
His post includes probing functions that Fusion 360 needs to use.
The one draw back that stopped me is that probing for F360 is part of the manufacturing extension and I just wouldn’t use it enough to warrant the expense.
Even using their token/credit system I’d have to drop $300 minimum a year for tokens that I would likely not completely use up before they expired (after a year).
This may already be common knowledge for folks in this thread but I did not see this angle discussed.
I’d strongly recommend looking at what David as published and using his post processor.
Hi David
A regular paid version of fusion includes probing for WCS, no extension needed…if you are using the free version it wont be there
The Machining Extension is no doubt way overpriced and I dont have it. What it allows is probing for inspection, which I dont do
However, even that can be accomplished by following David Loomes process that he outlined in a video he did on the subject
Here is a link to that
Ed
Hey Ed,
Thanks much for all the details, I think you covered it well Im sure I will have questions when I actually get into it, but what is the process at the machine and control? From what you said, you have to probe for the work offset the 1st time around, correct? SO what do you do from there? Do you just post out all MOPs, including the probing routines, and the control will prompt to load the probe like any other tool, then proceed with automatically probing Z, then X&Y, assuming that is the order I program and is obviously what we want, LOL?
Another BIG question is the practicality of using automatic probing for every setup. Can you use it to avoid manually probing the 1st time? "I thought there was some way to just post all MOPs with probing included and it would somehow magically probe WCS automatically? I was thinking that all you had to do was locate the probe tip in the approximate location, like you would do manually, from, say, the upper left corner, and then hit cycle start instead of using the probe page, you would just be running the program from the start. ?
Why is there no full tutorial on this from Tormach or AD?
I have a full license from my work I use for both work and personal work. Are you saying that David’s PP will allow all probing from Fusion without the need to pay for extras?
The manufacturing extension provides the full probing for inspection etc. workflow and tools. You can build a probing program just like you build a tool path.
I’ve got a single user license, it doesn’t come with the mfg ext.
Apparently from other responses, you can do probing with David’s PP without the extension.
Probably by using the standard “insert manual NC” in the setup builder.
Bill,
There are MANY videos on this topic, including this one that I did: https://www.youtube.com/watch?v=tNzjQv66zSM. Fusion is not the focus of my video but I go through and show the process of selecting features around 3:40.
You can use either the stock post with my probing routines or David’s post with his routines. The stock post is not able to do inspection, only setting work coordinates. I think setting work coordinates can be done without the extention, but that’s an Autodesk question. With either post set the work coordinate once yourself then the posted probing routines will be able to find the part.
Here are a couple other videos, if you want any additional ones I’d recommend searching “fusion probing” on youtube:
Thank you,
Norman
Thanks, Norman, I’ll take a look.