Simulation - Issues Dialog Box - Overtravel Warnings

[HarrisonClassic]

Hi.

I have been using the same machine and post library for ages, but I've noticed since the last few updates I've been getting this dialog box, even on files created years ago. 

What does it mean, where do I go to change settings to remove theses warnings? On some simulations there are hundreds of lines of warnings for X and Y....

[a.laasW8M6T · Accepted solution]

Hi David

The Overtravel warnings are coming from the way the Machine Definition/model has been set-up

The travel limits are set here for each axis in the Definition

They may be set incorrectly for your machine.

If you can't manage to get it figured out, you can share a file here that demonstrates the issue and we can take a look to try and solve the problem.

[HarrisonClassic]

Thanks

I changed the hierarchy of the axis to match what you have above - I get now Verification complete when I do a simulation.

Ta.

[bheskitt0806]

I have a Haas Tm-1p toolroom mill. I have a similar issue. Overtravel:Z warning when I try to simulate. As the original poster said, I am getting these warnings on old files that previously worked fine. I'm not sure how to properly modify my machine definitions, and wonder why they would have gone from working to not working. I hope to resolve this, but in the meantime is there any danger in running the code on my machine in spite of this warning? Thanks, Brian

[a.laasW8M6T]

Hi

If you want to share a file where you are getting the overtravel warning I can take a look and see what might be happening.

Generally the code for a 3 axis machine should be safe, your machine has its own soft-limits which will prevent overtravel's anyway.

The overtravel warning in simulation could be due to a number of reasons but unless you are running a very tall part with long tools, or a part close to the table with short tools you should be OK

[bheskitt0806]

Thanks for the reply.  I have attached a file.  I discovered that I get the warnings when I "simulate with machine", but not when I just "simulate".  Another thing that might be relevant, I had just downloaded the machine and post processor last week.  I did this because when I went to select a machine when I was doing a new setup, it didn't show up.  I had been storing my machine locally.  I forget the sequence of events, but in the end I downloaded the latest files.  As you can tell, I am a little foggy about dealing with machine and post processor files.  Some of my very old files use "Haas plain" as the machine rather than the specific Haas Tm-1p.  don't know if that is relevant.  Many thanks, Brian

edit: I was unable to send an example file.  the error I got:

Correct the highlighted errors and try again.

The attachment's instron sample.f3z content type (application/fusion) does not match its file extension and has been removed.

[a.laasW8M6T]

Hi

The Forum seems to be having issues with uploading .F3Z files.

You can get around this by butting them in a zip file and then attaching

[bheskitt0806]

thanks for the tip.  here it is

[a.laasW8M6T]

Hi

The issue is one of the scenarios I described earlier

Part on the table with short tools, so the machine actually is over-travelling.

From the Haas Website the Spindle nose to Table is 4"

Your tools Gauge length is

Your tool is going to 0.385" above the table.

4-(.385+3.449)=0.166" of over travel

If we move the part 0.2 off the table then we don't get an overtravel warning

Or if we put the tool in a longer holder or increase the stick out it goes away too.

So to conclude, Machine simulation is correctly detecting an overtravel condition based on the information you have given it

[nubrandao]

Hi, since you guys are talking about axis limit, I'm facing a problem.

I have program 2 parts in a DMG Mori Evo 80

I believe all the limits are exactly the same in the machine, related to eureka.

I have eureka in the company, but for now I can only run through powermill plugin to launch the machine and models.

In fusion when I simulate, I have no error.

When running in eureka, I have same times erros with Z axis limits, they seem to happen In tool change or at the begging of the next toolpath.

Not always. 

How to solve this? Change machine home 

position? Change the toolpaths heights doesn't seems to work.

[bheskitt0806]

Bless you sir.  Your explanation is very clear and makes sense.  I always ignored the part position tab of the setup dialog because I didn't know what it was for.  I think I have years of discovering details of this software to go.  Many thanks.