[stevieboy]

Hi guys,

I'm using Mastercam V9 and I'm wanting to run a mill that I've just bought off it. The mill is a Hurco BMC 20, I'm working in metric and I can send programs to the machine ok. What's happening is mastercam creates the programs with a decimal point in the feedrates, e.g. "F1500.0". The machine will not accept this and says the decimal point is "illegal". I can edit the program to remove the decimal points from all the feedrates before I send it to the machine, which isn't so bad for a small program but something big that needs drip feeding will be a bit of a hassle.

Is there any way I can set up Mastercam to not produce the decimal point in the feedrates by default.

Thanks in advance,

Steve.

[jackson]

Could it have anything to do with your baud rating ? i dont know about master cam i use Multi DNC for com. and i dont do metric

[psychomill]

Do you need to only have the decimal point removed? or also the "0" that's behind it?

I'm assuming you're using the Hurco post (MPHUR). If not, let me know, this may be slightly different....

Look in your post file and you should this:

# --------------------------------------------------------------------
# Spindle Speeds & Feedrate output formats
# --------------------------------------------------------------------
fmt S 3 ss # Spindle Speed
fmt F 5 fr # Feedrate
fmt F 11 fmod # Feedrate Modified
fmt 4 dirchg # Feerate Accel/Decel Flag
# ---------------------------------------------------------------------

On this line here...
fmt F 3 fr # Feedrate

Change the 5 to a 3. This will drop the decimal and any number behind it. It should post out a "F1500".

If you look above this in the post where it says "Format Statements", it should have a line like this:
fs 3 4 0

That should do the the trick. If not, let me know....

:cheers:

P.S. Make sure you make a copy of the post file first before you edit it. That way, if any mistakes are made and you can't get it corrected, you can still revert back to the original version to start over.

[stevieboy]

OK Psychomill, I'll give that a try and get back to you in the next few days. I'm not sure it'll work though but it's worth a try. It seems to be Mastercam itself that's the problem.

When I create a toolpath from a drawing the parameters box comes up to select the tooling. I pick the tool I want from the library and type in the box for the feedrate what I want it to be. Working in mm per minute so e.g. 500, 1000, 1500, etc. When I press enter Mastercam puts a decimal point in there followed by another 0, so 500.0, 1000.0, 1500.0, etc.

This then comes out in the program and the machine's controller won't accept it. I'll have a look over the weekend and get back to you.

Thanks for the help so far.

Steve.

[stevieboy]

Well I tried that and it worked, but only on feedrates with four figures or more, e,g, 1000 mm/min. For anything below that like a drill or tap routine that might have a feedrate of 500 mm/min it still puts the decimal point in there followed by another 0.

I don't think it's a post processor problem as this decimal point thing happens with everything else. In the toolpaths parameters dialogue box whatever figures I type in for any of the information, feedrates, depth cuts, stepover percentages, cutter diameter, it doesn't matter it still does it. I type a hole number with no decimal point and as soon as I press enter, bang, a decimal point and 0 on the end of it.

Any more ideas.:drowning:

[Matt Berube]

This can definitely be worked out in the post.

There is nothing wrong with Mastercam.

Unfortunately I don't know enough about posts to help you fix this.

I did notice that there was a similar question a while back...

http://www.cnczone.com/forums/showthread.php?t=27903

[ObrienDave]

Some of the text below blatantly stolen from psychomill's post.

stevieboy...
Try this...
In the MPHUR.pst file, you will find...

# --------------------------------------------------------------------
# Spindle Speeds & Feedrate output formats
# --------------------------------------------------------------------
fmt S 3 ss # Spindle Speed
fmt F 5 fr # Feedrate
fmt F 11 fmod # Feedrate Modified
fmt 4 dirchg # Feerate Accel/Decel Flag
# ---------------------------------------------------------------------

On this line here...
fmt F 5 fr # Feedrate

Make it read...
fmt F 10 fr # Feedrate

If you want to get rid of the decimal for drill cycle feedrates, In this section...
# --------------------------------------------------------------------------
# Drill variable formats
# --------------------------------------------------------------------------

look for...
fmt F 5 frplunge # Plunge feedrate in drill cycles

change to...
fmt F 10 frplunge # Plunge feedrate in drill cycles

Since none of the FMT lines are using FS 10, this will drop the decimal and any number behind it. It will post out a "F1500" or "F50".
Tested with MPHUR.pst
Works.

To quote Matt, "There is nothing wrong with Mastercam". Well..., sort of.

Normally, The input box data is "filtered" by the post processor.

The general idea of post processing is, so you can take a toolpath program from Mcam, run it through different machine post processors, and get the same result from different machines.

Post processors take care of different requirements for different machine and control combinations such as,

1. Tool change codes.
For example, I have a standard post and a different one set up to make the machine behave differently for extra long tools, or extra tall parts.
This can also take care of machines that require pre-staging the next tool in a dual arm changer, etc.

2. Arc center codes.
Such as, R or R- over 180 degrees, or absolute, incremental, or delta, I,J,K information.

3. End of program table movement.
I set mine up to retract the spindle and then present the table to the operator.

4. Axis letter data requirements.
Your machine control may not support decimal feed rates, others do.
Your machine may require different values for tool information, such as T6 H46 D46, etc., others may not.

The point is, it is the post processor's job to take care of these and other differences from machine to machine.

Please, don't be so quick to blame MasterCam.
Like any other tool, it is only as good as the person using it.

[Mike Mattera]

I have a free tutorial for this. Click the link below and then click "How To Edit A Post". It explains the Format Statement (fs).

http://www.mmattera.com/mastercam/index.htm

Mike Mattera

[stevieboy]

Hi Guys,

Well that seems to have done the trick so thanks a lot for all the help, especially you Obriendave, that sorted it, great. There's still a few things to sort out like the bore and drill routines. Also tool change positions for long tools/high jobs. There is a function for this in the machine's own parameters but I get a Y axis limit switch warning when I use it, obviously nothing to do with mastercam.

Your right, I shouldn't be so quick to blame the software, it's obviuosly just in need of the post setting up properly which is down to the operator. I guess I was getting a bit frustrated because it was doing something that I wasn't telling it to, but now I'm starting to see the bigger picture.

I'll be back on here soon with a new post for the other things but for now I'm a bit busy with loads of work to do.

Many thanks,

Steve.

[ObrienDave]

Steve,
No problem on the help.
I have found that there are a lot of very good people on this forum.
Most of us are happy to help simply because we have been through similar problems in the past.
I do it because I do not want to see anyone going through what I had to, to learn learn what I know.
Thanks for the chance to help.