Setup WCS with different Tool Orientation WCS

[Anonymous]

Hello! I'm trying to machine the side of a part that has already been machined on the top. A little info about what i'm using... I have a 3+2 axis CNC, but have to manually change the angle of the tool. 

My first image is my tool setup, with the appropriate WCS orientation that matches my machine's coordinate orientations. 

My second image is my adaptive clearing operation with a different tool orientation. 

I have read about Fusion allowing you to have different WCS orientations for the setup and tool orientations in the individual operations. Since I have to manually change the tool orientation on my machine, I need the setup WCS to mimic the orientations of my machine. I have tried to have my setup WCS and tool orientation WCS to be the same (as in my image #2) but when I load the g.code into my machine, it machines it as if I was machining the top of the part and not the side of the part. I would like to avoid having to reorient my part in my machine as that would cause a lot of clamping challenges due to the organic shape of my part.

Once I try to post using the setup and tool orientations in my 2 images, the post fails. Is there something I'm missing or am I going down the wrong path? I have also attached the .f3d file that my post is failing. Thanks! 

[RandyKopf · Accepted solution]

The WCS you established under the setup would remain the same. Use the same Setup for both tool paths. But each Tool path will have the Z Axis pointing in different directions.

So complete your first tool path from the top orientation as shown in the first image.

In the second tool path there is an option for tool orientation. Select a Z axis that is reflective of the second image. When it comes time to output tool path Fusion will see the difference in the setup WCS Z axis and the Tool path Z axis and know to rotate the machine accordingly.

The magic is using a single setup that defines you machines WCS. And each tool path uses a different Tool Axis Vector. That is the Z axis points one direction in the first tool path and another direction for the second.

I am not in front of Fusion at the moment or I would give you a screen shot of the Toolpath orientation screen. You will get a much more detailed response from the experts here before long.

Here is a link where I did something similar... 

http://desktopartisan.blogspot.com/p/pocket-ncs-home-position-with-respect.html?m=1

[Anonymous]

I got the idea of changing the z orientation between the setup and tool orientation from that exact post you attached in your response. I guess now my only problem is when I generate my code with the post processor, the file fails. I have attached a .txt file of the failed g.code I get from Fusion. (Actual file name that comes from Fusion is shoe_test-1.tap.failed)

[RandyKopf]

@Anonymous

Sorry my PC was down... It sounds like the post you are using doesn't support 5 axis. I would select a different post.

You can select the Pocket NC post when you choose to output tool path.

I've also attached a 5 Axis example it's 3+2 type programming. But it will show you the basics of setup and output using the Pocket NC post.

[Anonymous]

@RandyKopf the PocketNC post does not work with my Mach machine, even if I change the extention to .txt. Thanks.

[LibertyMachine]

Does it give you an error message at posting or when you run the code at the machine?

[RandyKopf]

@Anonymous

Understood the Pocket NC is a different machine. My suggestion was purely from the standpoint that is a working 5 Axis post. Just to test getting the program correct on the front end.

If it posts okay there you may need some help with your Mach post to get it to work. There are several people on this forum that can assist you with that.

Sorry for the misunderstanding!

🙂

[Anonymous]

@LibertyMachine 

When I try to post this toolpath with the generic mach3mill post, it gives me an error and I'm unable to get any post of out of it.

When I try to post this toolpath with PocketNC, it works but my machine will not load the toolpath.

After lots of research and reading, I need to modify the mach post to work with my machine. I just don't know how to do that (yet).

[Anonymous]

@RandyKopf It's my understanding I need to modify a mach post to get a vertical cut out of my machine. I just don't know who to go to or how to start modifying posts. I don't have a lot of coding experience.

[RandyKopf]

@Anonymous That is pretty clear what you need. The FUSION CAM file is probably good since you tested it with a working 5 Axis post. But it's clear you just need to get that Mach post modified to work. I know That @George-Roberts is pretty up to speed on posts or maybe Seth @LibertyMachinemight know who can assist as well.

[LibertyMachine]

What happens when you try to load the code? Have you tried re-labeling the file as a .tap? 

G-code is g-code, so it "should" work, although it's likely that there would be errors such as invalid G and M codes.

There are a couple other 5 axis posts available, I'm curious if those might be better to start with.

While @RandyKopf is right, in that you do need a post edit, it's often the case where it's easier to turn another post into a Mach post (or vise versa). So, can you cange the extension and report back?

[Anonymous]

@LibertyMachine I posted with PocketNC and changed the extension to .tap. When I load the code into my machine, I get M code errors and it won't load it.

[LibertyMachine]

Ok then, we're getting somewhere. Where? No clue, but it's progress 🙂

Could you once again change the extension to a .txt or .nc and attach the file here? For some reason, the forum doesn't support the attachment of .tap files (at least I don't think they do)

Tell me about your machine. Does it have a manual spindle on/off? What about coolant, vacuum, dust collector etc.

You say that you have to manually change the angle of the head. how is that accomplished? Any pictures of the machine you care to share so we can better understand what you are up against?

[Anonymous]

@LibertyMachine

I have attached the post that failed from yesterday's suggestion. Just to recap, I posted using PocketNC and changed the extension to .tap, and now to .txt to attach to this posting. I get M code errors when I load the post into my machine.

My code always has the feed rate and spindle on/off/speed included but the machine also has feed rate and spindle on/off/speed override. There's no coolant or coolant option. Since I only cut foam, there's a vacuum system attached to the wall (shown in the machine pic) so after (or sometimes during) machining, the scrap gets cleared off with the vacuum system. The close up pic better shows the geometry of the tool and holder. The whole holder rotates in increments of 90 degrees, then the tool rotates about a bolt 90 degrees to the "left" or "right." So, in theory, this machine is capable of vertically machining all for 4 sides of, let's say, a cube without having to rotate the part and re-clamping it. Also, of course, horizontally machining the top surface (which I can currently successfully do).

I start with gluing a foam block down to the concrete floor and machining the top surface so it is square with the machine (shown in the machine pic). Then, I glue my stock piece on top of the foam table and start milling. My end goal is to be able to tell the machine to cut side geometry vertically so I don't have to come up with complicated fixturing to get all sides machined. I primarily machine organic shapes.

I noticed in the code that posted from PocketNC, there's lines that say "A90. B0." which call for a table tilt. As shown in the machine picture attached, I do not have that capability. 

Hopefully this info helps you better understand my issue!

-Dezeray

[LibertyMachine]

Holy Cow! That's not a small machine!

By chance, did it give you any specifics on the errors? There are only a handful of M codes in the code you shared (0, 3, 5, 6, 9 and 30) so it won't be much work for you to find the offending one.

Getting a post to only post out the A rotation is no big deal. If we can narrow down what code is causing the error, we should be able to get you a post, either by modifying the PocketNC to work or the Mach3 post to work

Do note, I won't be able to pick away at this much during the day, but I can certainly sit down tonight and see if I can get this going. In the meanwhile, could you manually remove the M codes (except the M30) as well as the "B" callout and see what you can get?

[Anonymous]

@LibertyMachine

The error it gave me was "M0 error"

I also deleted all the M codes expect for M30, along with the lines with the "B" callout and had no errors. The problem was it started machining horizontally (XY plane) instead of the desired vertical (ZX plane).

[LibertyMachine]

@Anonymous I've not forgotten about this thread, I've just been super busy with work and family.

I've been mulling over your last statement " it started machining horizontally (XY plane) instead of the desired vertical (ZX plane)" and I've been trying to understand what you meant exactly. I think I've arrived at a conclusion, so please correct me if I'm wrong.

I've been looking at the code and your setup, and I didn't see anything wrong with it, the code should have been correct. It then occurred to me that perhaps your machine doesn't "know" that the head is tilted and you (and the machine) are expecting to see some form of "axis substitution" in the code, where what would be a "Z" move if done on the horizontal is now a "Y" move if done on the front and back sides. On top of that, if you are working on the left and right of the part, "Z" would become "X" and vice versa. Does that sum up your expectations and the machine needs?

IF that is the case, I'm afraid to say that this is way beyond my abilities. I could only hope to point you to a capable reseller who could modify a post for you. I'm honestly not even sure if it could be done.

If you are in the US of A, I highly recommend Silverhawk Solutions, as they've done work for me in the past and it's been top notch and very cost effective. But, before you go that route, I'd consider doing some digging and seeing if perhaps there is something inside of Mach3 that will allow for what you are doing. Are there other machines like yours out there that are able to do what you are looking for? Have YOU done what you are looking to do, only with another CAM package?

[Anonymous]

@LibertyMachine Yes, that is exactly what I'm trying to do. The machine doesn't know the tool orientation at all and there is no way to tell it that. You could say it's "dumb" in that way. So ultimately I'm needing a post modification to get the axis substitution. Thank you for taking a stab at my issue! 

To answer some of you questions, yes, someone else has been successful at the desired vertical cut with my particular machine. Unfortunately he uses RhinoCAM which we are not interested in because we run Mac computers and there is not and will not be a Mac version of RhinoCAM.

I'm just not understanding why Fusion would let you set up the tool orientation different from the basic XY (horizontal) cutting if it can't translate over to the machine.

I have reached out to Silverhawk and a few others that are suggested by Autodesk but I have not even heard from Silverhawk. That was about 2 weeks ago. Do they just take a long time to get a request going or am I inquiring in the wrong places? I simply filled out the form about modifying a post but I got no conformation email or anything from them.

[LibertyMachine]

The issue is that Fusion (and other CAM packages) want to machine with Z axis in-line with the spindle. Because your machine doesn't allow for spindle rotation (to my knowledge), it needs to be accounted for in the post processor, where Z becomes X or Y depending on the orientation of your head. Essentially, you need 5 different settings to account for, and that's assuming you only index your head(s) in increments of 90 degrees. 

My knowledge with Mach3 is MANY years old, so perhaps there is a way. I'd suggest asking over on the Mach3 forums: https://www.machsupport.com/forum/index.php and see if there is a method INSIDE of Mach3 that might allow you to avoid making a custom post.

Regarding Silverhawk, an email I use to contact them is: sales@silverhawk.us

[RandyKopf]

@Anonymous

Can you post a photo of your machine it might help @LibertyMachine or others...

It occurred to me that the part your doing is a little more complex with 5 Axis involved.

In the CAM learning world I found it best to keep things simple starting out.

That is make sure you got a solid grip on the basics...  

You are new to Fusion and CNC.

It might make sense to start with a basic 3Axis program to start out.

Maybe open one of the demo parts that is a simple 3 Axis. like I show in the screen shot.

This will let you see if your machine is behaving in normal fashion.

Second it will not confuse matters with extra 4+5 axis that are more advanced.

And post the output to see what you machine does.

Most 5 Axis CNC machines will default into a 3 Axis configuration.

You have to intentionally evoke the 4th or 5th axis by proper code output.

Just to rewind normally a 5 Axis CNC use a World Coordinate System to base all it's math output.

Typically running this type of machine in a 3 Axis mode it will use XYZ as a standard 3 Axis CNC.

I suggest opening Tutorial1_Complete provided with Fusion or any other 3 Axis file. The setup uses the WCS and each Tool Path Operation uses the same WCS for output. That means the Z Axis is always pointing the same direction.

And there is only 3 Axis output in the code that you would send to the machine.

If you post using the Mach3Mill that is provided with Fusion you should get standard 3 Axis output.

(1001)
(T1 D=50. CR=0. - ZMIN=-1. - FACE MILL)
(T2 D=8. CR=0. - ZMIN=-24. - FLAT END MILL)
(T3 D=5. CR=0. TAPER=118DEG - ZMIN=-25.502 - DRILL)
(T8 D=6. CR=0. - ZMIN=-24. - RIGHT HAND TAP)
G90 G94 G91.1 G40 G49 G17 (G17 is cutting on the XY Plane)
G21
G28 G91 Z0.
G90

(FACE1)
M5
M9
T1 M6
S955 M3
G54
M8
G0 X124.5 Y-44.092
G43 Z15. H1
Z5.
G1 Z4. F460.
G18 G3 X119.5 Z-1. I-5. K0. (There is a lead in move causing G18 output ARC on XZ Plane)
G1 X92.5
X-92.5
G17 G2 Y-4.658 I0. J19.717 (Normal output for this part is using G17 output ARCS on XY Plane)
G1 X92.5
G3 Y34.775 I0. J19.717
G1 X-92.5
G18 G3 X-97.5 Z4. I0. K5. (There is a lead out move causing G18 output ARC on XZ Plane)
G0 Z15.
G17
G28 G91 Z0.
G90

(2D CONTOUR1)
M5
M9
M1
T2 M6
S3000 M3
G54
M8
G0 X-96.68 Y36.31
G43 Z15. H2
Z5.
G1 Z1. F1000.
Z-23.2 F333.
X-96.673 Y36.312 Z-23.304
X-96.653 Y36.316 Z-23.407
X-96.621 Y36.323 Z-23.506
X-96.575 Y36.334 Z-23.6
X-96.519 Y36.346 Z-23.687

If you post this Tutorial1_Complete file using your post does it look basically the same? It should.

You can use this free tool to compare output from your post and the provided Mach3Mill post output

http://www.prestosoft.com/edp_examdiff.asp

will all that said your basic output using a 3 Axis