MASTERCAM AND LITTLE STOPS IN HSM

[batraul]

I have problems to mill in our HSC machine. I cannot reach feed rates of 160 inch/min without getting little stops in the machine. The machine uses Heidenhain TNC 430 and the chordal error I use (surface pocket roughing) is 0'0005. I've noticed that this stops are procuded mostly when the machine is making movements in all three axes. I make the .nc files with circle interpolations.

 

I thought there were too points that the control couldn't read and I tried to activate the option of filter arcs, but I don't know how it works exactly and decided to put a tolerance the double of the chordal error, a forecast of 100 lines and create arcs (forecast and arcs with default values).

 

Also the smooth tolerance for the machine (cycle 32 in heidenhain) was normal I think (0.002). But even doing this one the machine makes little stops.

 

What am I doing wrong?? Do anybody happened the same with mastercam?

 

Thank you in advance.

[Phil Orenstein]

I don't know about the Heidenhein control but I have encountered similar situations on my Haas with the Mpfan post. Firstly why do you need to have such a small chordal error of .0005 when you are roughing? I use .002 - .005 to avoid so many tiny movements. The stops may be caused by data starvation if you are DNC linking at a slow baud rate. I have experienced this data starvation at a baud rate of 9600 running finishing toolpaths at .0005 tolerance. To remedy this I had to slow down the feed pot to 35 IPM so the data could catch up. A faster connection might do the trick, say 34,8000 bps.

 

Hope this helps,

Phil

[Tony]

I have had one machine stop.It was the "job setup max feed rate for arcs" call out. In other words 100 ipm STOP,change feedrates for arc, 60ipm GO...

[Guest CNC Apps Guy 1]

This is NOT a Mastercam issue, it is a DNC issue. You cannot DNC at 100IPM with such small block movements. This causes data starvation as was mentioned earleir. The control is using the information faster than you are feeding it to the control so it has to wait until the buffer fills again so it can continue. You have 2 maybe 3 options;

 

[*]Get more memory for your machine

[*]Increase the baud rate (if it's not outside the distance limits)

[*]Connect the machine to the network.

[*]Slow your feed rate down on small moves

JM2C

 

[ 03-02-2002, 01:32 AM: Message edited by: James Meyette ]

[batraul]

First of all, thank you very much everybody for your help. I think this forum is fantastic and I can learn a lot here.

 

On the other hand, I will try to increase the baud rate of my machine.

What do you mean with "job setup max feed rate for arcs"? It's an option of Mastercam?

 

Which should be the parameters if I have to reach a tolerance of plus minus 0.01 mm?

 

Thanks to all

[Claus@Cimco]

Hi

Most Heidenhain tnc430 I know that are used for HSM, has a netcard installed and connects directly to the harddrive of a DNC computer through a NFS server. This way they can copy the NC-fil for the harddrive of the computer to the harddrive of the TNC430/426.

 

Claus@cimco

[Tony]

Your Right it is not a M/Cam issue.

It is my controller on that Machine.

Sorry if I confused anyone.

(We're on 40 with nothing to do but Qoute)

I'll stick to "Free cell" until further notice;)