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 make a feature request for a new Operation type? (WCS Translation/Offset)

edautodesk69XS4
Contributor

How to make a feature request for a new Operation type? (WCS Translation/Offset)

edautodesk69XS4
Contributor
Contributor

Hi, can someone point me to how I can make a feature request proposal to the Fusion 360 manufacturing team?

 

The proposal is a feature to translate WCS coordinates. This is fairly similar in UI (but quite different in outcome) to using probing where you click the "Override deriving WCS"

 

The purpose of the request is that many manufacturing shops will use a fixed reference point as their WCS origin to increase setup speed for many manufacturing jobs, for example the zero point location, point on a vice, corner of a jaw, etc. For example, in my case I use the top-left/bottom-right of the bed of each vice as a fixed reference point

 

However, this is inconvenient at the machine in as much as I much prefer the g-code coordinates to be relative to some point on the part itself, for example an underside face is generally my preferred reference. This has benefits in that I can quickly observe (at least in 3 axis machining) that Z axis references are all than xx millimeters above the zero plane, meaning I won't hit the jaws or whatever. Basically WCS relative to some distant point is hard to sanity check on the machine itself

 

On first inspection, the "Override deriving WCS" looks to do what is needed. However, it leaves the WCS based on the original WCS, so whilst it can correct for deviations between the CAD model and actual machine setup, it can't easily handle doing something like swapping out for a different set of vice jaws or moving the setup to a different vice altogether.

 

I can of course do what I need through a manual NC operation, but this is error prone if I change the CAD/CAM, then the changes don't flow through to the manual NC operation

 

The proposal is for an operation, which will need machine specific post support. It will assume that the user has created their setup with their desired on machine WCS, for example centred on the part. The operation will take a source point on the model and the source WCS that defines that point. This will work very similarly to how the probe UI looks today, except only points or planes would be selectable. The post will be responsible for setting the destination WCS to be equal to the source WCS, except shifted by the offset as measured from CAD.

 

The flow through the post would look very similar to the current probing code path

 

Opinions?

0 Likes
Reply
471 Views
7 Replies
Replies (7)

programming2C78B
Advisor
Advisor

I don't quite follow. Do you mean a translate? 

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

edautodesk69XS4
Contributor
Contributor

Hi, yes, that's correct (I thought I had used that term a few times in both the title and the description actually?)

 

To try and explain again, the key point:

- The machine has a fixed point defined on it, say G59 is the zero point fixture origin

- I want to create my machining setup such that the WCS is a point *on* the part itself. As an example, lets say I want to use G54 with the WCS based on a corner on the underside of the part

- (Reasons this is beneficial were discussed in the original post, but lets assume $reasons are compelling for the moment)

- The question is how to initialise the location of G54? 

- Note that the CAD model is assumed to exist and show the relative locations of G59 and G54, so we can click the measure tool and ask it for the incremental distances between those 2 points (in fact that is my current process today, I then manually type these into a manual NC command). However, the manual offset/translate process is potentially error prone and would not automatically update if the model changes

 

So the proposal is to add such an operation into the Fusion machining GUI. The workflow/UI would actually be quite similar to a probing operation. However, there won't be any real probing done, it's simply a workflow to establish the G54 WCS as being offset relatively from the G59 workspace (both arbitrary choices and only examples)

 

 

0 Likes

programming2C78B
Advisor
Advisor

I fully understand that now, I guess the question is why you would need this? If you already found your part g54, just run off that. If it's a repeat part, you can just save that translation distance from your known vice corner. 

I get you want to use the g59 to save time, but use g54 to be able to read the code "normally". In that case I'd just use a translation amount or decide if 2 minutes of finding g54 or being able to read code without math is worth more to you or the shop. 

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

edautodesk69XS4
Contributor
Contributor

Hi, I suspect you misunderstand the proposal?

 

When you reply "in that case I'd just use a translation", is exactly what the request is for. The ability to make a translation (meaning it doesn't exist in the Fusion Manufacturing GUI today).

 

Is this clearer now?

 

So I am requesting an "operation", whos purpose is basically to allow a GUI operation to translate the distance. Meaning, yes, i can write down those distances by hand, however, that's error prone, will not update as the model updates and the kind of crazy solution that logically ends with: Well, why do you need Fusion, just do everything by hand?

 

It's possible that the "just do the maths" bit is bothering you? The issue is the combinatorial explosion of jaws, machining positions, etc. I have only two double vices, yet I have a bunch of different jaws I can place in each position, each has a slightly different height, etc. It is certainly an old school method to write a setup sheet and expect the machine operator to diligently setup every machine to the micron. However, even that still doesn't allow for recutting some softjaws and replacing them, or a set of serrated first op jaws to be renewed (leaving to a z height shift) and it requires huge diligence from the operator. Similarly it doesn't provide a good solution to setting a workstop to place the part in precisely the required offset from a vice jaw side. In summary it doesn't scale well in my opinion

 

Consider Fusions current approach. I centre the part on the 1st op jaws, which means they are 24.252mm from the X left of the jaws. I have my WCS set to the bottom left corner of the vice say, which means that the operator needs to sanity check that they placed the raw stock at position X24.252, Y126.823, Z45.334 - this is not so easy, especially for that operator to check that the drilling op to Z45.433 is not going to colllide with the jaws or not?

 

The alternative is to build the job say referenced to the part corner/middle/etc. Now we drill to Z0.1, we move across the part from X0 to X100, etc. However, this part is in a WCS which doesn't exist in the physical space of the machine. So still we have a problem

 

My proposal to reduce the setup time on the machine and reduce error rates, is as per the original proposal. The part is programmed in a part specific WCS. However, that WCS is initialised based on an offset from a fixed point on the machine. Note that we use probing extensively and this is used to automate refining the final location of the stock, the initialisation simply needs to get us close. So this automates dealing with a softjaw being inserted differently and perhaps moving a few microns, or a workstop being set somewhat arbitrarily, or a 1st op jaw being replaced/renewed, etc

 

This immensely reduces the risk for me on setups, plus reduces the setup time. I can reset an old job without needing to scruitinise a setup sheet. Softjaws can be replaced and any relocation error gets compensated for. Workstops can be placed approximately and probed to initialise the job. Probing also helps reduce the error in say placing the part in the wrong vice, etc on the table. Yet also makes it feasible to swap the setup to a different vice with a small manual change to the NC code if needed.

 

There is a risk this proposal comes across as in some way complicated. I would encourge you to look at the existing functionality for  "Overriding WCS offset". This already works somewhat as above, only a) It doesn't solve the maths problem and b) only works for probing, it cannot be used for general offsetting duties

 

The problem with "the maths" is that your fixed reference point and the stock all exist in real locations on the machine. However, Fusion's "deriving WCS" ends up existing in a space which you can't see, touch or easily validate. The proposal here gives a way around this, which also updates as the model updates (eg you could swap in different vice jaws, re-create the softjaws in a new location, the posted code will automatically handle updating the offsetting of the WCS)

0 Likes

edautodesk69XS4
Contributor
Contributor

Perhaps a video of the desired use case is helpful:

 

* https://www.instagram.com/p/CusUIbRIfxk/

 

This is a job that requires several operations to run to very nearly full length of the tool and there is only about 1mm before collision with the tool holder. The operator needs to check the tool length before the job, we also automate the post to run a tool length check on the machine to hopefully spot a problem, then we use probing to ensure that the Z height of the actual part is used (as the part to part Z height will vary)

 

It is certainly possible to have the operator setup accurate work stops before this job. It would also be possible to cut accurate softjaws to hold this part in a precise orientation.

 

However, the trend in manufacturing is to reduce setup times, setup costs and improve accuracy. This is a low volume part and we were able to hold it in simple softjaws. We didn't even need to set a workstop (which on this part saves setup time as the part is quite tall and prone to tip and be non vertical if we use a workstop).

 

This part is programmed in Fusion, with the WCS on the top centre of the part, against the fixed jaw, which allows very simple sanity checking of the program delivered to the machine. The WCS for the part is initialised at the start of each run FROM the corner of the Vice TO an offset location on the centre of the fixed jaw. This offset is read directly out of the CAD/CAM for the job. The corner of the vice bed is fixed and will be reprogrammed if the vice is ever removed and replaced.

 

This WCS will be specifically incorrect for each part, X is offset because no workstop is used, Y is offset because a given softjaw is not the same width as another (to the micron), the Z is incorrect because it's standing on a tail of stock which pushes it to different heights. However, probing brings in the precise location of the part for each run of the part, and we can even put a thread into it which starts at a precise angle (which requires Z to be carefully measured)

 

The offset function in this case was extremely useful to ensure that job setup required little more than checking there were some softjaws fitted to the machine, no other WCS setup was needed. However, the program is error prone in that if if the CAD is changed, the person doing that MUST remember to also update the manual offsets entered at in the manual NC program at the start

 

I believe many shops refuse point blank to allow manual NC operations and so the proposal above allows for a simple way to setup the offset WCS, through supported GUI operations in Fusion.

0 Likes

DarthBane55
Advisor
Advisor

Hi, I see what you are after.  I wish I had that function as well, there are a few times I would have made good use of that.

 

On the same topic, if you have a machine which has a vise (for example) that never moves, you can output the offsets directly in the program.

For 3 axis machines, I think the math is from home, for 5-axis the math includes home position and center of rotation.  All this is done in the post, and it outputs G10 lines at the beginning of the program (assuming Fanuc controller).  There is such a function for all controllers I assume. For example, at the beginning of the program, the post outputs the following line:

G10L20P10X-13.6003Y-19.6388Z-18.4076A0.C0.

This established the work offset G54.1P10 (you can make it work for G54 of course, just need to look this up in the Fanuc manual).

 

For us, that means that any operation that is done on the raw material can just run, nothing to pickup (of course the position on the table has to be the same as in the software, so again, this is for fixtures that never move).  Any operation that is done on previously machined operations, we add a probe just to make the position super exact.  This is not useful for most people, but we use a lot of fixtures that are always on the same spot (think the Fifth-Axis vises etc).

I just thought I'd mention this in case it could apply to you, but I still would like to have the function that you described for sure!

0 Likes

edautodesk69XS4
Contributor
Contributor

Hi, see above. I already do a more advanced version of what you describe.

 

The problem with your approach is that the G10 is absolute to the machine. So if you replace the vice, then your G10 is broken.

 

What I do is run a Manual NC, which calls something like an incremental G10. So I have say P30 set to the corner of the vice. This will get reset if the vice is ever moved. Then I measure in CAD that the part will be incrementally offset X/Y/Z from that corner, and I run my macro to set this increment

 

This leaves me with

- a nice and easy to comprehend program in say G54.

- program is relative to G54.2 P30, so I only need to reset that if the vice moves

- Initial work offsets are set in CAD. This means one less thing for the operator to get badly wrong. However, it still leaves plenty of room for us to refine the position either manually on the machine, or using probing.

(Probing is amazing though. If you consider the workflow above, it means you can almost totally setup the machine from within the CAD/CAM workspace, even the machine offsets are initialised. Operator just needs to ensure vice jaws and tools are correct)

 

What I don't have:

- The offsets can get stale if the CAD is changed. There is no connection between them. Designer needs to remember to update them

- Offsets are manually entered. Especially as they can't be copied from the CAD workspace, this means they have been found through "inspect", written onto a post it, then transcribed into a manual NC call

 

If anyone wants my "offset WCS" macro, then happy to share. It's specific to Brother control, but should work on many Fanuc alike controls.

0 Likes