Clearance and Retract Heights, and Going to Z0 First Causes Collisions

[russtuff]

Hey crew, I appreciate any help you can offer, as I'm still learning and am not all that solid when it comes to offsets and heights. I am hoping someone can offer me some insight, as I am having issues with the code Fusion is generating for me (I post to LinuxCNC).

I may be misunderstanding the definitions I've found on the Fusion Help site for these heights, so I'll copy them first so we are all on the same page:

~ The Clearance height is the first height the tool rapids to on its way to the start of the tool path.
~ Retract height mode sets the height that the tool moves up to before the next cutting pass.
~ Feed height mode set the height that the tool rapids to before changing to the feed/plunge rate to enter the part.

In this shot you can see my part, the four slots I'll be pocketing, and the heights I have for this setup.

Based on the above definitions, here is what I expect to happen:

1. Rapid to Z3

2. Rapid to XY whatever

3. Rapid to Z.1 (the Feed height)

4. Feed into the first slot and do the job

5. Rapid up to Z.1 (the Retract height, which also happens to be the Feed height)

6. Rapid to the next XY whatever

7. Steps 4-6 until the fourth slot is done

8. Rapid to Z3 and end the program

My first problem is outlined in the code below, where we are going to Z0, then moving in the XY (crashing into the fixture), then retracting to Z3. Here is some sample code, and I have highlighted the movements to make it easier on the eye:

%
(POCKETING 4 SLOTS)
(T6  D=0.2187 CR=0. - ZMIN=-0.22 - FLAT END MILL)
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z0.
(2D POCKET 4 SLOTS)
N25 M9
N30 T6 M6
N35 S4600 M3
N40 G54
N45 M8
N55 G0 X-0.9606 Y4.9231 (crash)
N60 G43 Z3. H6
N65 G0 Z0.1219
N70 G18 G3 X-0.9818 Z0.1 I-0.0219 K0. F24.
N75 G1 X-1.18 Z0.0931
N80 G17 G3 Y4.8269 Z0.0878 I0. J-0.0481

the program goes on and on

My second problem is that after doing the first slot, instead of retracting to the Retract height and rapiding to the next slot it is retracting to the Clearance height. This isn't a major issue, and only a little inefficient since we are moving at rapid speed anyway. Here is a screenshot of the simulation where I would expect to see the movements between slots happen at Z.1, but they are happening at Z3:

My third (and final) problem (and now I'm really being picky), is at the end of the program we are at Z3 from the final retract, but head back to Z0. It makes more sense to me that it should stay up at Z3 so I can change setups. I always just delete that part of the code, which you can see here:

program has been going nicely....
N1115 X-4.3347 Y4.9264 Z-0.211 I0.0121 J-0.0182
N1120 X-4.3367 Y4.924 Z-0.2049 I0.0158 J-0.0151
N1125 X-4.3373 Y4.9231 Z-0.1981 I0.0178 J-0.0127
N1130 G0 Z3.
N1140 M9
N1145 G53 Z0. (I always remove this line)
N1150 M30
%

Thank you anyone who can explain or help.

[HughesTooling]

For some controls G53 moves are absolute machine coordinates so to Z0.0 would move to the Z home position. Has your machine got limit switches and are you homing the machine at start up.

Mark.

[LibertyMachine]

russ, welcome to the forums and Fusion!

 What sort of a machine are you tring to program, CNC router, retrofi manual mill, desktop mill?

Looking at your code, I'd like to point out a couple things:

N20 G53 G0 Z0. THE POST PUTS THIS IN BY DEFAULT. As Hughes stated, it's a move to home switch and/or tool change location
(2D POCKET 4 SLOTS)
N25 M9
N30 T6 M6
N35 S4600 M3
N40 G54
N45 M8
N55 G0 X-0.9606 Y4.9231 (crash)    THIS ISN'T A CRASH MOVE. The machine is still at Z home
N60 G43 Z3. H6                     This move is a rapid move to 3" above the part, activating the Height offset 6
N65 G0 Z0.1219                     This move is a rapid to .1219 above the part
N70 G18 G3 X-0.9818 Z0.1 I-0.0219 K0. F24.            This move is an arc in the G18 plane onto the part at Z.1 (I disable this output, waste of code and unneeded)
N75 G1 X-1.18 Z0.0931                                And from here on, it appears taht it's ramping into the slot

[LibertyMachine]

Are you using the stock post processor? If so, I/We can edit it and have it not post out the G53 moves, that's easy stuff

[jeff.walters]

If your working on a PC when you post there are options on the lower right of the post window. If your machine dosent play well with the G53 then you can switch it to use the the G28 insted. 

[russtuff]

---

@HughesTooling wrote:

For some controls G53 moves are absolute machine coordinates so to Z0.0 would move to the Z home position. Has your machine got limit switches and are you homing the machine at start up.

Mark.

---

I had a feeling this queuestion was going to be asked and if my post didn't already feel so long I would have gone into it. I don't have limit switches wired up yet, and I'm homing it by myself.

Thanks.

[russtuff]

---

@Anonymous wrote:

Are you using the stock post processor? If so, I/We can edit it and have it not post out the G53 moves, that's easy stuff

---

Yes I am using the stock post.

[russtuff]

---

@Anonymous wrote:

russ, welcome to the forums and Fusion!

 What sort of a machine are you tring to program, CNC router, retrofi manual mill, desktop mill?

Looking at your code, I'd like to point out a couple things:

N20 G53 G0 Z0. THE POST PUTS THIS IN BY DEFAULT. As Hughes stated, it's a move to home switch and/or tool change location
(2D POCKET 4 SLOTS)
N25 M9
N30 T6 M6
N35 S4600 M3
N40 G54
N45 M8
N55 G0 X-0.9606 Y4.9231 (crash)    THIS ISN'T A CRASH MOVE. The machine is still at Z home
N60 G43 Z3. H6                     This move is a rapid move to 3" above the part, activating the Height offset 6
N65 G0 Z0.1219                     This move is a rapid to .1219 above the part
N70 G18 G3 X-0.9818 Z0.1 I-0.0219 K0. F24.            This move is an arc in the G18 plane onto the part at Z.1 (I disable this output, waste of code and unneeded)
N75 G1 X-1.18 Z0.0931                                And from here on, it appears taht it's ramping into the slot

---

Thanks!

I'm using a benchtop mill I converted to CNC. It is starting to sound more and more like this is an issue with my not having limit switches wired yet. I guess I'm gonig to have to get on top of that ASAP to see if it solves some of these issues.

[russtuff]

---

@jeff.walters wrote:

If your working on a PC when you post there are options on the lower right of the post window. If your machine dosent play well with the G53 then you can switch it to use the the G28 insted. 

---

I have not noticed that, and I'll double check it right away. This would probably solve my problems for now, until I get the limit switches wired.

Thanks!

[LibertyMachine]

Many years ago, I built a tabletop CNC router pwered by Mach3. I cannot advise you enough to look into limit switches. Poor machine did so many overtravels so many times in it's infancy. We're talking hard overtravel errors. Simply not good for mechanical motion controls to reach the limit that mine were. Lesson learned.....

[russtuff]

---

@Anonymous wrote:

Many years ago, I built a tabletop CNC router pwered by Mach3. I cannot advise you enough to look into limit switches. Poor machine did so many overtravels so many times in it's infancy. We're talking hard overtravel errors. Simply not good for mechanical motion controls to reach the limit that mine were. Lesson learned.....

---

I know exactly what you mean, as I've fought some of those same issues. I'll move it up on my priority list. 

[russtuff]

---

@jeff.walters wrote:

If your working on a PC when you post there are options on the lower right of the post window. If your machine dosent play well with the G53 then you can switch it to use the the G28 insted. 

---

Hey Jeff I looked for this but didn't see it. I'm sure it's obvious, but can you throw in a screenshot?

[russtuff]

---

@russtuff wrote:

---

@jeff.walters wrote:

If your working on a PC when you post there are options on the lower right of the post window. If your machine dosent play well with the G53 then you can switch it to use the the G28 insted. 

---

Hey Jeff I looked for this but didn't see it. I'm sure it's obvious, but can you throw in a screenshot?

---

I found what Jeff was mentioning, but it isn't in the window when you post process. I had to click the "Open config" button then within the Brackets windows I found:

var useG28 = false;

I've read over how LinuxCNC handles G28 and it doesn't look like the solution I am looking for in this case.

Thanks for the help everyone.

[jeff.walters]

Russ have you emailed cam.psosts@autodesk.com? If not plese do they can help you get your post to what you need. 

[russtuff]

I have not, but I will.

Thanks!

[Anonymous]

Hi all - 

Was wondering if anyone could share the fix for this issue. I'm running into the same exact problem.

I am also using LinuxCNC v2.5.4 and encountering issues with travels of the z-axis, where the start of the run has the bit drag across my stock. The only fix I've been able to gather (from this helpful post) is to change this (N20 G53 G0 Z0.) to something like (N20 G53 G0 Z0.2). Having the post processor do this automatically would be immensely helpful as I’ve ruined a few pieces and bits from forgetting to modify the code before my runs.

I am using the default configured EMC post processor in Fusion 360 on a home built XYZ machine. 

Regrettably I am also running into a plethora of other z-axis problems where my z-axis is offset some weird distance. I suspect it has to do with my misunderstanding of the heights within Fusion 360, but I'll dig into those issues after fixing this one. A sample of my nc file is attached. 

Thanks for any assistance!

[russtuff]

I sure haven't found a way around it. In your example of N20 G53 G0 Z0, I just change it to something like N20 G0 Z1 at the beginning of the file and delete the G53 line at the end of the file.

This issue seems to stem from not having home/limit switches set up on the machine. Oh well for now I guess.

[HughesTooling]

If you go to this link I've put up some info on how you can set the home position from the post processor properties when you post.

https://camforum.autodesk.com/index.php?topic=7032.msg30642#msg30642

You could also request a modified post from cam support.

Mark

[Anonymous]

Rus and Mark - thank you both!

While I wasn't able to get Mark's modification to the emc.cps file to work I was able to make some serious progress. In fact I've learned what was causing my z-axis to act so wonky and I'm back in action with Mark's suggestion of modifying the post.

The suggestion of modifying the post ultimately led me to the LinuxCNC forum, in particular http://www.linuxcnc.org/index.php/english/forum/search?q=emc.cps&childforums=1 where I found some useful posts from others.

The posts suggested Fusion CAM adds odd code (nothing personal Fusion Gurus) - and indeed that is what helped isolate my wonky z-axis, which turns out to be a separate issue than the Z0 this post is about. I had unknowingly correlated the wonky Z-Axis to the start of the bit being down at z0. I kept trying to compensate my machine and as a result, ran into weird behavior. Because the tooling in Fusion Cam has an offset, that I didn't notice after the recent upgrade my machine wouldn't cut or would start moving before getting above the workpiece, breaking my bits. The tool offset and my monkeying with machine offsets was causing my Z-axis to travel way too high or not high enough depending on what I was milling. I (stupidly) kept choosing different tools - not paying attention -  with different offsets in trying to isolate the problem. I've been stumped since the recent upgrade to the tool selection in CAM.

I had created custom tooling in the previous Fusion CAM and removed the offset on my mills. With the upgrade the offset in tooling is back and my custom tools have gone missing. Looking through my machine file carefully I found G43 codes. Removing those and My Z-axis is on mark again (no pun intended). I guess for now I'll live with the manual modifications to the z-axis (which have always been there) and play around some more with the post configuration. While I can follow some of the code in the emc.cps file there are no comments to reference. If I figure out how to get Mark's suggestion working I'll most certainly share.

Thanks for the help and all the Best,

Gene

[g.awada]

hey 

reviving an old post since I could not find a solution. I have the exact same problem. I set my mill at the very top of the stock and the machine drags it along the stock to the milling start point, then it goes up to the retract height (after scratching the surface) and back down to the cutting height, which makes absolutely no sense! I searched high and low but could not stumble across a solution other than setting it up high enough so it wont scratch then manually setting it down once its about to start cutting. I know there is a fairly simple setting that needs to be tweaked but I just cant find it. 

I'm using GRBL post processor from OpenBuilds on a home built cnc machine.

any and all help would be appreciated. 

thank you.