G53 Z0. when changing work offsets

[miller391]

I am running a haas VF3 and i have 4 identical parts on the table so i am using the multiple work offset in the post process. I am wondering if there is a way i can control the z retract height when the machine changes work offset. Now it is using a G53 Z0. line at the end of each offset code. The Z does not need to retract to home each time as it adds alot of time to my cycle time. Im sure there is a way to edit that hoping someone will have the answer.

Thanks!!

[Anonymous]

You'll want to open up your program and edit it manually.

I've asked and the only way to do this is to 

G0 G90 Z1.0(or your requirement there)

Make sure after you put in another G90 G0 and the offset

G0 G90 ZX.X

G0 G90 G154 P2

[Anonymous]

Or you could do a 

G28 G91 Z1.5

then

G0 G90 G154 P2

Depending too, you might have to put in a 

G01 Z.25 F20.0 HXX

[DarthBane55 · Accepted solution]

You can definitely do that in the post, all of our posts have the mod done, but it is quite involved and above what I can do in a post edit.  I can tell you that it involves creating a "manual NC - Action", and then a lot of checks in the post to know if you are just jumping part or if you are at end of tool etc.  I'm just telling you this because the other person here said that the only way was a manual edit, but I know for sure you can do that in the post, I just can't help you getting that done...   In fact, you can almost do anything you want in the post.  You should get in touch with a post editor master dude that is listed in the sticky section at the top of this forum.

[Anonymous]

You're probably 100% right, but at the end of the day, Fusion360 should be able to do that without all the challenges and editing.

I don't know why when you tell fusion "hey im doing more than 1 part" on that Setup Tab portion, why doesn't it give an option to force a "new" clearance height of X.X" inches or MM when going in between parts? Fusion already recognizes to send the spindle home in-between work offsets, so why not have an option to force the spindle to go up "ZX.X" in between parts and on the last op of that tool, then send spindle home with a "G0 G53 ZX.X".

They don't do it because they said it could cause a crash and if you want to do it, you have to do it manually. I've already asked about a post being modified for this, and Fusion wouldn't touch it because of the crash issue.

[DarthBane55]

Yes it is true that it could cause a crash.  I can understand their view on this, they cannot take that risk.  

We use a gcode simulator (NCSimul) and have a "private" post master guru that has done all sorts of really fun stuff for us, but we see in the simulator if the output will crash or not.  For the masses, I understand what Fusion did, because you could have clamps and what not between 2 parts, and if your machine does "dog leg" rapid moves, and fusion doesn't do that, you could crash and you would not see it in fusion.  There are many ways to crash if they built that function in.  Don't forget that Fusion also aims at hobbyists that might not have a very good understanding of the gcodes.

[miller391]

Okay Thanks! Thats why i cant find alot of info on it cause its not easy to do. I have been editing the programs manually but if i had to tweak the program and reload it from my computer it would change my manual edits in the program. I figured there would be a setting to change but guess not. Thanks for the help anyway ill see if i can get intouch with him and see if i can change it. Thanks again!

[seth.madore]

---

@DarthBane55 wrote:

..if your machine does "dog leg" rapid moves, and fusion doesn't do that, you could crash and you would not see it in fusion.  There are many ways to crash if they built that function in.  Don't forget that Fusion also aims at hobbyists that might not have a very good understanding of the gcodes.

---

Dog-leg rapid is a Haas problem, not Fusion. Fanuc had the smarts (for once) to provide for a parameter to cure for that issue. Haas, not so much 😉

And actually, the post edit is rather simple (or at least it used to be a couple years ago when i did it to mine). Not sure what else would need to be solved for to handle Manual NC and all those checks you mentioned @DarthBane55 

[DarthBane55]

By the way, when do you a change in Fusion, you can keep all your edits...  use a file compare program, you put the new posted file beside the old one, and transfer only what is needed, keeping all your edits.  the file compare program highlights only what differs in both files, makes it super simple to keep your edits.

[DarthBane55]

Hi Seth,

didn't mean to say that dog leg rapids was a problem, just a difference, and if a user is not aware he can crash easily.

For the post edit, there might be an easy way, but we use it for 5-axis machines, and it involves not only part to part, but index clearance moves etc.  It is quite complex in our post as it verifies a lot of stuff.  We have a different retract between parts than for index, etc.  But for 3 axis machines, maybe it is simple.  Was just trying to say that it's doable in the post, and that I, cannot help to do the change (above my head in post editing).

[seth.madore]

Gotcha! Yeah, 5 axis and retracts is a whole other ball of wax also way above my head. 3 axis was absurldy simple, I thought there had to be way more to it than that.

Not sure if that's still the case, they've reworked the posts many times over and it may not still apply.

But yeah, the issues you state are valid and you are correct, Autodesk is not thrilled with providing the means to a serious crash.

Ever see a 4" facemill sheared right off? It ain't pretty..

[DarthBane55]

---

@seth.madore wrote:

Ever see a 4" facemill sheared right off? It ain't pretty..

---

Lucky for me, no! 😮

[ifuASTJY]

This has been implemented in the generic Brother post.

I wish all posts have this!

It's a must!

I tested this today, works perfect.

It needs implementation  on all posts please.

[ifuASTJY]

[Anonymous]

I see you posted a screenshot of the Brothers post with the Clearance option. How close is the Brothers post to say the NON-NGC HAAS post?

[seth.madore]

Sweet Mother of God.....

I'm gonna ask a few questions....will post back in a bit

[ifuASTJY]

We only run Fanuc, siemens and brother( whic is pretty much fanuc ISO), I have no experience with Haas, but one should try to edit the existing Haas post ( which i guess is optimized for Haas machines).

I guess will have an answer soon 🙂

@seth.madore 

[seth.madore]

Good news!

The post team does have plans on adjusting the more common posts (Haas, Fanuc etc) to include the same ability as what is now in the Brother post, in regards to multiple WCS and retracts. It's on their list, but I don't have a timeframe to share.

So yeah, it looks like we managed to find a solution that doesn't immediately open users up to high risk crashes 🙂

[ifuASTJY]

@seth.madore  Any news on the Clearance Height Retract selection for Fanuc, Siemens, etc...?

It's been a while 🙂 

Thanks

[seth.madore]

I've not heard any news on this front, sorry.