4th axis workflow and concepts

[LibertyMachine]

Hello all,  (this might be is a long post, you've been warned)

I am posting this in the HSM forum as there are more actual machine shop programmers and machinists in this forum than there are in the Fusion CAM forum where I spend the most of my time.

My machine is a 3 axis mill (Mori) with a 4th axis mounted along the X axis. I have a plate that I can affix a vise or chuck to and use it for 3 sided machining, or mount a spindle nose to the 4th and gain access to 4 sides of a part (with proper workholding, of course).

In Fusion, (and Inventor as far as I can tell) I have two options for setting up, say, a job in a vise, on my 4th. I can use Tool Orientation and select the proper face to indicate which surface I am working on, or I can have individual Setups for each angle I am working at.

If I use Tool Orientation, I am finding that my initial work offset of G54 is carried throughout each tool and angle. The A callouts are correct, but the G54, in my mind, should not be applied to every operation.

If I am at A0, I would use G54. If I rotate forward to A90., I'd want to use G55, and if I rotate backwards to A270., I'd use G56.

Moreover, with Tool Orientation, my XYZ coordinates are all coming from my initial G54.

For instance; if I was to drill a hole in the top of the part, at A90, I would expect the code to look something like this:

T1M6(.250 OHD)
M11
G0G90G55A90.X0.Y0.S2500M3
M10
G43H1Z.05M8T2
G81G98Z-1.R.05F5.
G80
M9
G0Z.05
G49G53Z0M19
M1

It's actually giving me something closer to this:

T1 M6 (.250 OHD)
M11
G0 G54 A90. X-.3536 Y-.2714 S2500 M3
M10
G43 H1 Z3.45 M8 T2
G98 G81 Z3.3711 R3.45 F5.
G80
G0 Z3.45
M9
G49 G53 Z0. M19
M1

Those values are coming from the the 3-axis distance from G54. It makes sense, I suppose, if I was using known center of rotation. But in reality, I'm not. That workflow is great when you have dynamic work offsets (I don't), or the work is generous enough with tolerances to allow for minor discrepancies throughout the machining process (it's not). The use of additional work offsets allows me to be very precise in locations and compensate for part deflection, machine growth (warmth) and other issues as they arise.

Now, the OTHER method is that of having multiple Setups. This sort of works, although it has problems, which I'll describe best as I can.

While it gives me the proper XYZ dimensions, all the A values are zero. G54 A0, G55 A0, G56 A0., so on and so forth. Yes, I "could" adjust the A offset in my control to reflect the actual location, but I'm wondering if that's the only way...

Moreoever, to have an involved job with 60 operations, 28 tools, all doing something at each new angle, that is a cr*p ton of Setups and it becomes such a cluster...fudge to go through and work on.

So, I need to understand workflow in this area. I am not at all opposed to working with a reseller to modify my post to more accurately reflect my process and intent. But I need to know if I'm going about this in the proper fashion and there are other methods I should be considering.

Thank you for all those that actually followed this to the end!

[Steven.Shaw]

hmmmm, what about using a folder and overriding the work offsets?

I believe what would make this easier is operation specific work offsets, Correct?  

[LibertyMachine]

I ran a part not too long ago. I can't publicly share the file, but I can do a screencast and select sharing via email. It's one of the more involved 4 axis jobs I've programmed in Fusion.

I tried Folders. The issue I ran into is that I could not get the flow I needed. Ideally, T1 would have started off at A0, went to 90, back to 270.. With Folders tool changes were all over the place and I could not find the proper sequence of things.

That job became such a chore to make sure everything was flowing as it should for least amount of wasted moves and decent efficiency throughout. I know there has to be a better way, I just need a nudge in the right direction.

The method that I employed reminds me of my MasterCam days. It was FAR from efficient

[LibertyMachine]

In Esprit, you would have each work offset in a Setup. In each of those would be your toolpaths in whatever manner you programmed them. Totally irrelevant to the outcome. You had a second tab that you can drag operations up and down and re-order everything. Not saying that is the best manner, it's an option.

In Fusion, I can see making a Setup for A0, another for A90., and yet another for A270.. But, how do you go from that to a program that actually makes any production sense? You would have to have A90_1, A90_2, A90._3 so on and so forth. It's absurd to think that is the process.

[Laurens-3DTechDraw]

There is a reorder to minimize tool change in the post dialog.

This would help if you go the multiple setup way.

[Laurens-3DTechDraw]

But what I personally would do if I had the same issue as you do is make a fully custom post.

Where you just use one Setup. Select the new coordinate system for each tool orientation.

Then the post can be made so it doesn't remap the coordinates to the original Coordinate System(like default).

And have the post check all the orientations, output these in an interactive window, where you can give what work offset from the machine you want for what A-axis rotation.

That's what I would do. But that serious post editing, after that, it's very convenient to use I think.

[LibertyMachine]

I agree, @Laurens-3DTechDraw about using one Setup. It's much more straightforward and less prone to confusion.

I think I've lined up a reseller who will do this work for a reasonable price. I'm not at all opposed to spending money. My time is better spent keeping my machine(s) running, programming my next job, inspecting parts. I edit what I can, and realize my current limitations.

That being said....

Select Coordinate System in Fusion (or Inventor Pro). How does it work, how is it supposed to work? Selecting that option, it looks like the software wants me to select something, but I have no idea what. "Coordinate System" is what appears under the mouse if you let it be for a moment. Where do I click to establish my next CS? Clicking on anything bumps me back into "Select Z and X axis"

Is this currently not an option, although it's on the roadmap for either product? I'm ok with it not being fully functional on the software side, although it does make it difficult to develop a post with software limitations..

[Laurens-3DTechDraw]

I live in the HSMWorks world of things so there it's really easy to make an coordinate system in solidworks.

But you don't have to.

You would be able to use the select Z and X-axis.

But you would have to place the Origin on the place of your machines work offset.

Like you can here:

[LibertyMachine]

Alright, I think I understand that. So, while it's posting out numbers relative to my initial Setup (currently), the post should be able to be modified to reflect positions relative to that Tool Origin that I now select during the Tool Orientation process. That makes sense. 

However, by what method do I define that origin as G55, 56 etc? If it's all in one Setup, it's going to want G54. Unless there is something that I'm missing...

I need an HSM dev in here, lol

[Laurens-3DTechDraw]

---

@LibertyMachine wrote:

Alright, I think I understand that. So, while it's posting out numbers relative to my initial Setup (currently), the post should be able to be modified to reflect positions relative to that Tool Origin that I now select during the Tool Orientation process. That makes sense. 

---

Yes, exactly that.

---

@LibertyMachine wrote:

However, by what method do I define that origin as G55, 56 etc? If it's all in one Setup, it's going to want G54. Unless there is something that I'm missing...

I need an HSM dev in here, lol

---

Then my method would be for the post to open up a window for you when you have clicked post. Where it shows all the A-Rotations it finds in the machine where you give in what G54,G55,G56 would be used for what A-axis rotation. That was my idea.

[LibertyMachine]

I've been thinking about this issue, off and on all day. The post edit you suggest would be a solution, yes. If I can convey that to the reseller and they don't flip a lid and double the price....well, that's a different deal.

@al.whatmough Is it possible that the dev team has plans in store for Tool Orientation improvements? It seems to me that it might include a button to override the current WCS? I could make an IdeaStation post if anyone else thinks they would benefit from this added flexibility. The lack of other people chiming into this thread suggests I might be the odd duck.

[Laurens-3DTechDraw]

---

@LibertyMachine wrote:

@al.whatmough Is it possible that the dev team has plans in store for Tool Orientation improvements? It seems to me that it might include a button to override the current WCS? I could make an IdeaStation post if anyone else thinks they would benefit from this added flexibility. The lack of other people chiming into this thread suggests I might be the odd duck.

---

Well I think you are. And future wise more and more machines will have dynamic work offsets, so it might become even rarer. But who knows maybe a lot of people are actually looking for this now.

[Steven.Shaw]

its worth a shot, I know some other users on here with older horizontal machines would appreciate it. 

[LibertyMachine]

Well, I put an idea up on the IdeaStation.

Laurens, while I do agree that dynamic work offsets and machine intelligence is the future, there are an unbelievable amount of older (or more basic) machines on the market and they will continue to be there for decades to come. It would make sense (in my mind anyway) to meet the needs of that large segment, provided it is a prudent usage of developers time.

[Greg_Haisley]

I have to agree with @LibertyMachine there are a lot more older machines than new. So pleasing the few with dynamic rotation should be a secondary request.

The use of folders with WCS control seems to be the answer with this UI with tool sorting based upon the user's preference. In part that  @LibertyMachine posted. The roughing out of all sides then finishing would be the best approach IMHO. So you would have 2 folders for each angle, one to rough out and one to finish. Personally angle control has not been an issue for me. Rather sorting the out the program and understanding which tool to adjust for a feature size is more important. You could have the length of a facing tool cause a feature on the side to be out of position relative to the face mill length for example. So do you adjust the WCS for the side or adjust the length offset for the face tool? This can be a real problem for operators that don't understand what the program is doing.  It's like playing a game of chess. One move may affect many other future moves.

[LibertyMachine]

To the second point of your statement, regarding what do you adjust;

I would say that there are two types of CNC machinists. The "operator machinist", who needs to be presented with the most foolproof and simplified process, and the full fledged machinist who can make very good parts out of even the most complex of setups. Because let's face it; there is so much going on with a 3 axis vertical being made to perform work to all sides of part, lack of dynamic work offsets, crash detection and all the bells and whistles that come along with the new, nice machines. I would say that I am in the second group. And the work that I do would only really suit that same group.

Folders are nice. And they could possibly be the solution. However, what do you do when you need to have a roughing tool come in a second or third time to fulfill another role? What about a finish tool that runs several times at multiple angles? What if you need to have (for whatever reason) T17 come in before T5?

If there can be a method to closely adjust the post process output to accurately reflect what is needed, I'd support that as equally as WCS control at tool orientation. Selecting "Re-order tools to minimize tool changes" did not give me what I needed. The only thing I found that worked was the fiasco that you saw in my screencast. Many setups only leading to confusion. And this wasn't actually a complex part, it just had enough going on at every angle

[Laurens-3DTechDraw]

@Greg_Haisley @LibertyMachine

I would have to disagree this is an old machine problem. Tilted work plane command has been available on Fanuc, Heidenhain and siemens controls for decades. It's more that people didn't buy the option on the machine and still want to do 4-axis or 5-axis work. Which I understand but it's not that the machines, control or CAM-Systems are to blame. It's more that the buyers of cnc machines tend to be bad at looking forward to their future needs...

Whereas on a lot of machines's it would be possible to buy the option afterwards, yeah costs money will be worth it in the end.

But I do agree putting some time in to get this right could help a lot of people, I'm not sure if they(those users) would actually recognise that.

[Greg_Haisley]

I am soooo old that I remember the time when helical milling was an option. A $2500 option in 1981! The Fanuc tech came in and switched a parameter on and we had helical milling. The owner was not a happy camper let me tell you. 

@Laurens-3DTechDraw you are absolutely correct when it comes to selecting the control options. Typically the owner would be the last one involved with the control option selecting process. He typically is all about saving money. So control options that may or may not be ever implemented is where the owner is coming from.

@LibertyMachine the machinist (group 2) that totally understands the programmer's concept of how to process a part are few and far between. They are like dinosaurs, almost an extinct species. I could go alot further on this subject but I better not.

[LibertyMachine]

You are right, those options do exist in some (most) of the older machines. But as you said, they are $$$ when bought after the fact. When I bought my Mori, I had a long list of things I "wanted" but really had to pare it down to what I needed. Doing anything else would have significantly raised the monthly payment and was not a step I was willing to take, just setting off on my own. The last 8 years of my day job and dealing with Esprit, I saw the simplicity of the code output and how it needed a folder for each angle, but allowed independent ordering of toolpaths in the exact manner needed, and I'm just looking for ways to bring that function into HSM.

Still looking for a dev (cough @al.whatmough cough) to chime in and indicate the direction of this conversation. If it's dead in the water, I'll accept that and just let this thread die a peaceful death.

[LibertyMachine]

---

@Laurens-3DTechDraw wrote:

---

@LibertyMachine wrote:

Alright, I think I understand that. So, while it's posting out numbers relative to my initial Setup (currently), the post should be able to be modified to reflect positions relative to that Tool Origin that I now select during the Tool Orientation process. That makes sense. 

---

Yes, exactly that.

---

@LibertyMachine wrote:

However, by what method do I define that origin as G55, 56 etc? If it's all in one Setup, it's going to want G54. Unless there is something that I'm missing...

I need an HSM dev in here, lol

---

Then my method would be for the post to open up a window for you when you have clicked post. Where it shows all the A-Rotations it finds in the machine where you give in what G54,G55,G56 would be used for what A-axis rotation. That was my idea.

---

So, I'm working with a reseller to implement these changes to the 4th axis post. Specifically, calculating the XYZ relative to the Tool Origin that I select in the Tool Orientation process. I suspect that they might be struggling with implementing this change, as the last post I tried out from them was not even close to what I was looking for. I've not even asked about a pop-up window, just looking for the tool origin at this point.

@Laurens-3DTechDraw do you have any suggestion as to what should be coded in to make it behave like this, or should I kick that over to the Post forum...