Tool orientation, does setting a new origin actually work?

[vworpi]

I think I've tried everything with this one. If we set tool orientation on a toolpath and select a new origin, Fusion always seems to ignore the new origin and sets the CAM figures relative to the setup WCS origin. Surely setting a new origin point should create a new xyz datum?

I've had a look at the post setting here, and that doesn't make any difference. Am I missing something obvious?

I've previously been setting angular datums via an additional setup & tool orientating each tool in that setup to gain the correct B axis position. The additional setups WCS is set to the origin point I want to datum from.

Today I've been trying to use folders instead, overriding the work offset number and (as before) tool orientating each tool to get the correct B axis position.

[seth.madore]

Have you gone through and edited your post processor as described in the linked article?

Yes, the post can be made to output a new XYZ value via "selected point", as this is the method I also use for my 4 axis programming. I'm disappointed that I don't have the option of assigning new G5x values, outside of using multiple setups...

[vworpi]

Yes, I've made the two alterations from the article. I'm using a modified post based on the generic fanuc post supplied with fusion. I've had multi axis (in my case B) running fine for a couple of months.

[vworpi]

So, you're getting a new origin with "selected point" rather than any of the other options? So, select z&X, origin from sketch point? I tried box points after my post mod.

[seth.madore]

I've always been using "Selected Point" and setting a Sketch point to wherever I need it, such as center of a bore, intersection of a couple features etc.

Just testing now, and it also works fine with Model or Stock box points

[vworpi]

I'm still not seeing this post out correctly with the post mods applied.

I've attached a simple demonstration of what I'm trying to achieve. Do you want a copy of my modified post to peruse? I'm wondering if I have some settings clashing in there.

[daniel_lyall]

What is the error saying when you post the model it should work.

[vworpi]

No error message. It produces a working program, but where I'm expecting the G55 face to post out with the hole centre being X0 Y 0 Z0, it's actually X15 Y0 Z15

What I want:-

M22
G90 G00 B[#601+0.]
M21

G54 G90 G00 X0. Y0. S5000 M3
G43 Z101. H1 T0
M8
(SEQ - DRILL1)
G00 X0. Y0.
Z21.
G98 G81 Z-15. R2. F1000.
G80
Z101.
G91 G28 Z0.
G49

M22
G90 G00 B[#601+90.]
M21

G55 G90 G00 X0. Y0.
G43 Z101.
(SEQ - DRILL2)
G00 X0. Y0.
Z21.
G81 Z-15. R2. F1000.
G80
Z101.
M9

What I get:-

M22
G90 G00 B[#601+0.]
M21

G54 G90 G00 X0. Y0. S5000 M3
G43 Z101. H1 T0
M8
(SEQ - DRILL3)
G00 X0. Y0.
Z21.
G98 G81 Z-15. R2. F1000.
G80
Z101.
G91 G28 Z0.
G49

M22
G90 G00 B[#601+90.]
M21

G55 G90 G00 X15. Y0.
G43 Z116.
(SEQ - DRILL4)
G00 X15. Y0.
Z36.
G81 Z0. R17. F1000.
G80
Z116.
M9

[seth.madore]

Can you share your Post Processor here? Not sure if cps files are still allowed for attachment, so you might have to dump it in a zip file and attach that instead

[vworpi]

There you go. 

[vworpi]

Did you get a chance to have a poke at my post?

[daniel_lyall]

It is the center of rotation, it being out by 15 it is 15 away from the setups WCS.

If you have the WCS dead center of the model in the setup and then in the second toolpath you have it in the same places with the Z pointing in the correct direction it works fine. 

[vworpi]

Yes, we know this. The issue is that tool orientation "origin" is not actually creating a new origin, it's always referencing the original setup WCS origin.

This is apparently possible, but doesn't appear to work with the recommended post mods.

[daniel_lyall]

I have never seen it work or seen someone get it to work with an offset with a standard machine.

[seth.madore]

@daniel_lyall  it does work, I've got it going on my Fanuc post.  The only issue I have is that everything comes out with a G54 offset and I need to do a Find+Replace (CTRL+H in Windows). But regarding XYZ values coming from "Selected Point" and using Tool Orientation, yeah, it does work.

I've just not had time to focus on this post and dive into it. I will try to set aside some time for this one, my apologies...

[daniel_lyall]

So you want a G-code output like below but I am not 100% sure it is safe to use the code below I have no real way to test it.

%
<1001>
(MC4)
(PART NO:)
(DRG DESC:)
(OPNO:)
(JIG:)
(REV:)
(ISS:)
(MATL:)
(CYCLE TIME:)

G90 G94 G17 G49 G40 G80
G21

M0
(NOT PROVEN)
(ADD WORK OFFSETS HERE)

#601=0.(INITIAL B POSITION)

G91 G28 Z0 M19
T1 M6

M01
(10 DRILL)

M22
G90 G00 B[#601+0.]
M21

G55 G90 G00 X0. Y0. S5000 M3
G43 Z31. H1 T0
M8
(SEQ - DRILL5)
G00 X0. Y0.
Z21.
G98 G81 Z0. R20. F1000.
G80
Z31.
G91 G28 Z0.
G49

M22
G90 G00 B[#601+90.]
M21

G56 G90 G00 X0. Y0.
G43 Z31.
(SEQ - DRILL6)
G00 X0. Y0.
Z21.
G81 Z0. R20. F1000.
G80
Z31.
M9

G91 G28 Z0.
G49

M22
G90 G00 B[#601+0.]
M21

G91 G28 X0 Y0 Z0 M19
M01
M0
M98 P9901
M30
%

[daniel_lyall]

Yep, I forgot that I have done it before took a bit to remember and dynamic offsets.

I just prefer to use a center of rotation then the toolpaths can carry the orientation.

[seth.madore]

Center of rotation is perfectly fine when you are machining everything together and your workholding will never change, such as a dovetail fixture. Once you start adding in such things as removable vises and chucks, things start to really move around and you kinda need the flexibility of defining multiple WCS systems. Unfortunately for us, Fusion isn't really setup for this sort of thing without a fair amount of post tweaking....

[daniel_lyall]

I have had times when having the origin where you want it to be would make stuff a lot easier to do, having to offset stuff gets risky at times.

[vworpi]

---

@seth.madore wrote:

@daniel_lyall  it does work, I've got it going on my Fanuc post.  The only issue I have is that everything comes out with a G54 offset and I need to do a Find+Replace (CTRL+H in Windows). But regarding XYZ values coming from "Selected Point" and using Tool Orientation, yeah, it does work.

I've just not had time to focus on this post and dive into it. I will try to set aside some time for this one, my apologies...

---

No apologies necessary. 🙂