Chief Designer

[mitchghmgarage]

Fusion 360 creates an improper tool path with violent spindle crash into work at 650 IPM.
See attached Fusion 360 program a resulting tool path. It appears that:
1. Line 2455 issues G49 command cancelling tool length compensation.
2. Line 2460 issues G0 Z-.5 which without tool length compensation crashes tool, tool holder and spindle into work.
This is also true for lines 6855 & 6860, 11270 & 11275, 15680 & 1568.

It is interesting to note that lines 20075 & 20080, 24095 & 24100, 28070 & 28075, and 32145 & 32150, 36202 &36210 and 40190 using a different sequence:
1. Issues G49
2.. Issues G53 G0 Z2.5
Given the lack of tool length compensation I believe this scenario will also cause the same disastrous results.

I tested the first rotary tool path in air and mistakenly assumed that the remaining would also work properly - shame on me!

I am NOT sure that my tool strategy did not cause this improper tool path, but the simulation looks fine.

[johnswetz1982]

If it looks fine in simulation but something goes wring at the machine that is probably going to be a post issue. What post are you using? Is it a stock post or modified. Please attach the post you are using.

[mitchghmgarage]

<meta charset="UTF-8" />

[daniel_lyall]

---

@mitchghmgarage wrote:



<meta charset="UTF-8" />

---

???

[mitchghmgarage]

I tried to Post this out yesterday, not sure what happened, but here it is again:

All,

Thank you in advance for your help!

I was using the attached Post called "haas next generation 1-20-2021.cps" .   It is the HAAS NGC post I  downloaded on December 20.  It was three days old at that time.   It has one modification which I made after I received the error below while making a different part.  

“Rewind of machine is required for simultaneous multi-axis toolpath and has been disabled.”

The modification was made in accordance with an entry on Autodesk Knowledge Forum.   See link below:

https://knowledge.autodesk.com/support/autodesk-hsm/troubleshooting/caas/sfdcarticles/sfdcarticles/H...

You can find the modification I made by searching the Post file  "haas next generation 1-20-2020.cps" for the comment "Mitch Gross".  In addition, I used a parameter setting "SafeRetractDistance" of 1 when I generated the G-code.  I thought that should be sufficient and not run into problems of over travel in the Z axis. 

To make sure the modification or this Post file was not the problem, I downloaded the latest Post file from Autodesk, reran using this Post file (unchanged) and have received the same bad G-code,NC file.   I have attached this Post file as well.   It is the file named "haas next generation 1-28-2021.cps".  

I have also attached the resulting NC file with the bad G-code tool path created using the brand new, totally unmodified Post which was the same as the NC file created using the December 2020 Post file. 

Here is  my take on the G-code that the Post creates.   For some reason, as you can see, at the end of the tool path (.5 Rotary6 2) Block 2455  has a G49.   This cancels TCPC, but  G49 also cancels tool length compensation.   The next block then has a G0 Z-0.5 which with tool length compensation off sends the spindle careening into the work.   Bear in mind that in order for the rotary tool path  to clear the part holding fixture with the C axis at 90 degrees the tool holder is 6 inches long with 2 inch tool length for a total of 8 inches.   So, the spindle does not have to travel far at 650 ipm to crash. 

Like wise, the second set of Rotary tool paths have equally bad G code, and  it causes a Z axis over travel.  At the end of the tool path (.5 Rotary6 2)  block 20075 the Post  uses a g49 to cancel TCPC, the next like has G53 Z2.5 which cancels tool offsets and work offsets and attempts to move to Z2.5, which on a HAAS UMC750 is not a valid machine offset position.  There are similar problems with the end of this tool path at lines 24095 and 24100 and at the end of all the rotary tool paths in the NC file. 

I know and have manually fixed all these problems.   However, what this means is that every time I make a change to the part design or any other tool path change, I have to remake all these changes and then check and double check to make sure no errors are introduced.   This is very time consuming a negates the reasons for having a CAM program in the first place.

Mitch

[engineguy]

@mitchghmgarage 

Forgive me for joining your conversation as I am very confused, you mention that the problem code is not recognized by the UMC750, I am able to Post code here without the G53 Z2.5 problem code you are getting using the HAAS UMC/750 Post Processor 🙂

Yes, there is a G49 at the end of every Operation and that is what I would expect as every Operation has the following code at the beginning of each new operation :-

G28 G91 C0

G90

G53 G0 Z0

Followed by :-

 M11
 M13
 G0 B**. C**.
 G234 H8

 And then carries on with the toolpath for that operation

So, that says to me that the machine is moving to it`s Machine Z0 to be safe after the G49 command and as you can see there is a new G234 H8 tool length offset command so all that should avoid any crashes!!

I do not see anything wrong with the code as it is here, I am only able to Post for operations that use the same tool with the Personal use version but what I have Posted does seem to be OK to me 🙂

@daniel_lyall 

and

@johnswetz1982 

Daniel and John please have a look at the attached code and see if I have got this correct, you both have more experience on this stuff than me, happy to be wrong if that`s the case 🙂 🙂 🙂

Probably miles off but at least I tried HAAS UMC/750 PP used is attached 🙂 🙂 🙂

Stay Safe

Regards

Rob

[daniel_lyall]

Can you do a screenshot of the toolpath properties you have set? also does G28 work better for you than G53?

This is a pain G53

This code temporarily cancels work coordinate offsets and uses the machine coordinate system. This code will also ignore tool offsets. In the machine coordinate system, the zero point for each axis is the position where the machine goes when a Zero Return is performed. G53 will revert to this system for the block in which it is commanded.

[engineguy]

@daniel_lyall 

Easy enough to select the "Use G28 instead of G53" option at point of posting and there will be no G53 commands in the code at all so that should be a quick fix, yes ?????

Might have to change the onClose section to unlock the 4th and 5th axis again before all the axis Zeroing ???

Stay Safe

Regards

Rob

[johnswetz1982]

I wasnt going to mess with this, just figured that posting the post processor would speed up and trouble shooting. I also would not be running any unproven program at full rapids either.

[mitchghmgarage]

Hi All,

Using G28 instead of G53 is worth a try, just not sure of any other ramifications.   One thing for sure is it will reset the trunion unnecessarily to C0 and B0 only to move it right back again.  I will have to check out other ramifications

.  

We did test the code in the air at slow speed through the first rotary roughing pass and it ran fine.  We then mistakenly decided the rest would run correctly.  Shame on us, lesson learned.  

Two much more experienced G code programmers than me have looked at this G code and cannot understand why the Fusion 360 post file was written in such a way that it would create this code. It does not seem to understand where the spindle/tool is relative to five axis positioning.  Also not clear why it turns off TCPC when the next tool path is another rotary using the same program zero.   I guess the post is not forward looking.  

Not sure what screen shots you would like me to make.  So please let me know what you would like me to post.   However, as I am currently watching the snow pile up, I will probably not be at work until late Tuesday or Wednesday.  

Thanks,

Mitch

[mitchghmgarage]

Not sure what Post processor you are using, but the latest and greatest from Autodesk for the HAAS UMC machines is what I used.   The G49 is used for some reason to cancel the TCPC, but the unintended (I hope) consequence it is to cancel tool length compensation.  The next block has a G0 Z-.5 which has three problems.   One the part is still rotated and the trunion is at B90. Two, the c axis of rotation is at the center of the rotated part  (essentially in the X direction) which has a 2.250 inch diameter.  Therefor Z-.5 is close to the center of the solid part.  So, this code tries to ram the spindle through the center of the part.  Three,  it cancels the tool length compensation for a combined tool holder and tool that is eight inches long.   Also a recipe for disaster.  

Not sure where the  other blocks you reference are in the program, but this tool strategy has ten roughing passes to remove material from an undercut geometry.  Ideally, rotary would have roughing and finishing passes, but I do not believe it does.   Let me know if it does because that would make life much easier.  So we created them by issuing ten separate rotary tool paths each leaving progressively less material until it is ready for the finishing rotary pass. 

If there is a better way to accomplish this, please let me know.  

Thanks,

Mitch

[mitchghmgarage]

PS.  The code is in fact recognized by the UMC 750, it is just that the code created has the UMC 750 do very bad things.  

[daniel_lyall]

A screenshot of the settings you are using in the pre-post dialog will help to have it apples to apple, it is a guess at the moment, there are the other settings in the pre-post dialog that affect it as well.

[mitchghmgarage]

Attached are the screen shots of the Post Processor settings I use to generate the code.

Thanks

[mitchghmgarage]

Hi,

Setting "safe retracts"  to G28 instead of G53 I think works for the "second" set of five rotary tool  paths, in that it no longer over travels the Z axis.

However, the first set of five  rotary tool paths are still a problem and result in a crash.  The code for the first set remains:

N2455 G49 (TCPC OFF)

(.4 Rotary6 3)

N2460 G0 Z-0.5

N2465 G28 G91 C0.

[daniel_lyall]

Reading through posts with a problem that is basically the same on a Haas machine G254 DWO comes up as an issue it would not hurt to try it in an air cut.

[engineguy]

@mitchghmgarage 

Here is some code that I am getting, does it look better like this ???

N4445 X-2.5596 Y-0.6858
N4450 G49 (TCPC OFF)

(.4 Rotary6 3)
N4455 G0 Z0.9985
N4460 G28 G91 C0.
N4465 G90
N4470 G53 G0 Z2.5

It has almost an inch clearance which should be enough for the C axis to go to C0, yes ???

If so then after the C0 movement it goes to G53 G0 Z2.5 which again should be fine as that is 0.25in more than the 2.25in Radius of the part ??

Stay Safe

Regards

Rob

[mitchghmgarage]

Hi Rob,

The problem I believe is in these two sequential blocks of code you listed:

N4450 G49 (TCPC OFF)

N4455 G0 Z0.9985

According to page 360 of the UMC750 Programming guide page 360:

"These ... program codes cancel G234 (TCPC)...:

G43 - Tool length compensation + 

G44 - Tool Length compensation - ,

G49 -  G43/G44/G143 Cancel."

Here in lies the problem.   It seems the Post uses G49 to turn off TCPC.  Unfortunately, the unintended consequence is it turns off tool length compensation as well .  The tool and holder together protrudes about 8 inches below the gauge line to clear the trunion of the UMC750,  but even if it were shorter, say 2 inches including the tool holder,  block 4455 would cause the tool and spindle to go crashing into the work and beyond as long as work offsets are still in effect, which they are.   This behavior has been confirmed by what the machine actually does with these commands - air cutting of course.   I am not the worlds greatest G code programmer, but I believe the machine is behaving as expected.   Let me know if I am wrong and there may be a wrong setting on my machine.   I do use all the "default" machine settings and have always thought they would be correct - but maybe not. 

I am hoping maybe someone on the forum has a work around for this problem other than manually coding a fix every time I post out this setup.  It would make life much simpler, since this and other problems with Posting out five axis Rotary tool paths seem to be pervasive.  Maybe even a tool path other than Rotary to accomplish the same thing.   I have contacted Fusion 360 Tech Support and they seem to think there is a problem with the Post processor and have turned this over to Development for evaluation and fixing.  Unfortunately, there is no way to contact Development so I do not know the status of a fix.   I suspect I will not see much until a new release of the software sometime in the future.

Best regards,

Mitch

[daniel_lyall]

Have a google of this Haas G254, it seems to be a common problem even in Mastercam.

@seth.madore  Do you know anyone who can help with this? 😁

[mitchghmgarage]

Hi Daniel,

I looked at Google for HAAS G254 and only saw one problem on VMC machine, not UMC 750.   Am I missing the Google items to which you are referring?  Can you please point me to more listings on Google.   I am trying to learn how this all works - very confusing. 

Also, I think the problems I am having are more related to G234 - TCPC than HAAS G254 - DWO.  The rotary tool path I am using is really 4 axis to which G254/G255 DWO enable/disable do not apply, I think? 

Thank you and best regards,

Mitch