Haas Mini Mill Tool Change Table Offset

[andy_concept303]

Hi all

I’m fairly new to CNC machining and Fusion 360. I have a job to machine that is quite tall but within the scope of the Z machine capacity. However, the tool change procedure occurs at a much shallower Z compared to the top of the job, which would result in a crash.

What I would like to do is move Z all the way up, and X all the way over to the right, then do the tool change.

I’ve done a bit of research and seen mention of setting 210 in the control (normally zero) which I assume would provide this offset, but after changing it to -405.0mm in X, it has no effect.

The job incorporates two WCS origins.

Is there a way to command this Z and X move before the next tool change operation from within Fusion? I’m aware of the manual NC function, but not familiar with it. I guess editing the code manually is another option, but again not something I’m very familiar with.

Thanks in advance for any help.

Andy

[Matthew-R]

@andy_concept303 Thanks for posting this question to the Fusion 360 forum. It sounds like this issue could be remedied with a post processor edit. That being the case, I'm going to move this thread over to the post processor specific forum. Out post experts should be able to help you better with this issue. Thanks!  

[andy_concept303]

Great thanks.  I did read an old post where someone had done that to addresss a similar issue, but was for a different machine and don't think it was resolved.

[keith_clausen]

Hi Andy,

It is a pretty simple post edit that I have done for my mini-mills. I would be happy to share and or do the edit for you if you would like.

I would need two things from you, the post you are using and the maximum positive Z axis can travel.

Basically The way my post works is that it uses G53  to move the Z axis to the highest it can go (this is a bit different on every machine) when a tool change is called prior to calling, the X axis to move as far it can move in a negative position (basically moving the job as far away from the spindle), then the Z axis will drop to the tool change position, do the tool change and then move to the Maximum Z position prior to any XY movement to get back in the cut.

While this adds more over all movement to you programs it is the safest way of doing it with these machines and frankly any machine with an umbrella carousel.

[andy_concept303]

Hi Keith, that's really kind of youm thanks so much!  I'm not very knowledgable in this area so may need you to walk me through it if thats ok?  Will check those travel limits tomorrow and get back to you.  Thanks again.  Andy.

[keith_clausen]

No Worries Andy. Happy to help. I look forward to getting the information. Regarding walking you through anything, let me know.

[andy_concept303]

Sorry, meant to say, when you say 'post', do you mean the actual G-code program or which post procrossor I'm using?  If the latter then it will be the "HAAS (pre-NGC) / haas".  Thanks.

[keith_clausen]

Yes I meant the actual Post Processor.

So you are just using the generic un-edited Haas post processor for the legacy control. So In that case all I will need is the maximum positive Z axis position to code it into the post. Are you familiar with what I need and how to get that? 

[andy_concept303]

Yep, just using the generic one in Fusion 360.

Just nipped out and checked my machine (2008 Mini Mill)

Max X travel to right is: -406.400mm

Max Z travel height is: +112.235mm

This what you need?

Thanks.

[keith_clausen]

That is what I need. Do you only use the machine in metric?

[andy_concept303]

Yep! No inches for me! 🙂

[keith_clausen · Accepted solution]

Here is a modified post. The G53 positions for XYZ are hard coded for the retracts. There is a more elegant way of doing this but it should work for you. It has for me for the seven years I've been running mine.

I've take a look at the posted code as should you....please test the post.

Here is a small snippet of code so that you can see the retracts and positioning.

%
O00001
(Using high feed G1 F5000. instead of G0.)
(T1 D=38.227 CR=0.381 - ZMIN=0. - bullnose end mill)
(T2 D=14.478 CR=0. TAPER=45deg - ZMIN=-1. - chamfer mill)
N10 G90 G94 G17
N15 G21
N20 G53 G0 Z0.

(Face1)
N30 G53 G0 Z110.0
N35 G53 G0 Y-1.0 X-406.0
N40 T1 M6
N45 G53 G0 Z110.0
N50 S1015 M3
N55 G54
N65 G0 X71.424 Y-18.455
N70 G43 Z15.24 H1
N75 T2
N80 G0 Z5.334
N85 G1 Z3.874 F508.
N90 G18 G3 X67.602 Z0.051 I-3.823 K0.
N95 G1 X47.847
N100 X-47.847 F762.
N105 G17 G2 Y14.309 I0. J16.382
N110 G1 X47.847
N115 G18 G2 X51.669 Z3.874 I0. K3.823 F508.
N120 G0 Z5.334
N125 G1 X71.424 Y-18.455 F5000.
N130 Z3.823 F508.
N135 G3 X67.602 Z0. I-3.823 K0.
N140 G1 X47.847
N145 X-47.847 F762.
N150 G17 G2 Y14.309 I0. J16.382
N155 G1 X47.847
N160 G18 G2 X51.669 Z3.823 I0. K3.823 F508.
N165 G0 Z15.24
N170 M5
N175 G53 G0 Z0.

(2D Contour1)
N185 G53 G0 Z110.0
N190 G53 G0 Y-1.0 X-406.0
N195 M1
N200 T2 M6
N205 G53 G0 Z110.0
N210 S4021 M3
N215 G54
N220 G17
N225 G0 X-46.755 Y39.209
N230 G43 Z15.24 H2
N235 T1
N240 G0 Z2.54
N245 G1 Z0.448 F381.
N250 G19 G2 Y37.761 Z-1. J-1.448 K0.
N255 G1 Y36.313
N260 G17 G3 X-45.307 Y34.865 I1.448 J0.
N265 G1 X45.307 F508.
N270 G2 X48.982 Y31.19 I0. J-3.675
N275 G1 Y-31.19
N280 G2 X45.307 Y-34.865 I-3.675 J0.
N285 G1 X-45.307
N290 G2 X-48.982 Y-31.19 I0. J3.675
N295 G1 Y31.19
N300 G2 X-45.307 Y34.865 I3.675 J0.
N305 G3 X-43.859 Y36.313 I0. J1.448 F381.
N310 G1 Y37.761
N315 G19 G3 Y39.209 Z0.448 J0. K1.448
N320 G0 Z15.24

N325 M5
N330 G53 G0 Z110.0
N335 G53 G0 Y-1.0 X-202.0
N345 M30

%

If this solves your immediate issue please offer some Kudo's and set to solved.

[andy_concept303]

Many thanks Keith.  Have downloaded the file, could you advise how I call it up in Fusion?

[keith_clausen]

You can either upload the post processor to Fusion or keep it local. If you keep it local you can specify the path and post in the post processing Dialog during posting. If you want to upload it to the cloud the post needs to be the CAMposts folder in Assets.

[andy_concept303]

Sorry, I meant how do I reference / use it in the Fusion post processer window, do I browse for the file in the highlighted box? (see attached)

[keith_clausen]

Hi Andy,

I think I know what the issue may be. You have uploaded the revised post to you Assets/CAMpost folder but can't se how to select the Cloud Post that you uploaded in the post dialog during posting. Is that correct?

[andy_concept303]

Errrr no, but I think I fudged my way through it....

First I browsed to my new (local) .cps file using the Configuration Folder box (I didn't click on the Setup box), and ran the post processor, and it seems to work OK i.e. the code looks good, not run machine yet.

But, then I lost the path to all the generic processors!  But, now found them again.

So, would I normally copy the new file into the folder containing all the generic Fusion ones?

i.e. C:\Users\*****\AppData\Local\Autodesk\webdeploy\production\5669a8135e51a5c306a7cdb9b99cf334ce773328\Applications\CAM360\Data\Posts

Guess it doesnt really matter as long as i know where it is!

Thanks again, and sorry for all the spoon feeding!  Only started using Fusion about a month ago....

Andy

[keith_clausen]

If this is the case, but you are not seeing "Use Cloud Post" as an option to set the path, then you need to enable "Enable Cloud Libraries" found in "Preferences". You may need to restart Fusion once enabled. 

[keith_clausen]

---

@andy_concept303 wrote:

Errrr no, but I think I fudged my way through it....

First I browsed to my new (local) .cps file using the Configuration Folder box (I didn't click on the Setup box), and ran the post processor, and it seems to work OK i.e. the code looks good, not run machine yet.

But, then I lost the path to all the generic processors!  But, now found them again.

So, would I normally copy the new file into the folder containing all the generic Fusion ones?

i.e. C:\Users\*****\AppData\Local\Autodesk\webdeploy\production\5669a8135e51a5c306a7cdb9b99cf334ce773328\Applications\CAM360\Data\Posts

Guess it doesnt really matter as long as i know where it is!

Thanks again, and sorry for all the spoon feeding!  Only started using Fusion about a month ago....

Andy

---

If you are storing and accessing custom post locally I would not place them in the same folder as the installed generic post on the off chance the name of the *.cps files are the same because when Fusion updates you could have an over-write issue wiping out your modified posts. 

I'm pretty particular about house-keeping in these regards (posts, tool libraries, operation templates etc.) and keep it all separate from the installed default folders. Even if the post has not been modified I will just copy it to a new location keeping it separate from the default install folders. 

[andy_concept303]

Thanks, yeah, just been playing around with those locations, and moved it out and into the personal folder.

Funny you should mention the icloud libraries, i just ticked that option earlier today and intend to get my tool library etc uploaded to the cloud.