Rhinocam 2 and Mach3 Problems

freshwatermodels · Post by **freshwatermodels** » Tue Mar 03, 2009 12:59 pm

Has anyone had problems using Rhinocam2 with Mach3???

I started with Rhinocam but recently tried using the new Rhinocam 2 and am having problems.

In Mach3 I am having problems with either everything locking up or getting a condition abnormal > " Exact Stop vs CV Mode"

Any one know how to deal with this???

Post by **MecSoft Support** » Wed Mar 04, 2009 4:02 pm

We have not heard of such an issue. Can you contact Mach3 and see if they can figure out what is going on?

freshwatermodels · Post by **freshwatermodels** » Wed Mar 04, 2009 5:18 pm

I asked about this on a Mach3 forum. One said that a G64 is missing and another said he wondered why the R0.1 is in the code. I think there may be conflicts in the code but I'm not good enough at G and M code to trouble shoot this. I tried both the version 1 and version 2 posts and had same results. I am wondering if I did something wrong so will redo the part and see what happens when code is posted.

Rhinocam was very well suited to my needs and I wanted to keep current and bought the new Rhinocam2 . Now I wish I had the old version running to make parts while I try to figure out the problem.

Jack

G00 G49 G40.1 G17 G80 G50 G90
G20
(Standard Drill )
M6 T1
M03 S4583
G00 Z0.1250
X0.5000 Y0.2810
G81 X0.5000 Y0.2810 Z-0.6 R0.1
G80
G00 Z0.1250
G81 X2.0000 Y0.2810 Z-0.6 R0.1
G80
G00 Z0.1250
(2 1/2 Axis Profiling)
M6 T2
M03 S2000
Z0.0935
X1.5875 Y0.6880
G01 Z-0.1000 F20.0
X1.5833 Y0.7408 F6.0
X1.5710 Y0.7923
...........
X0.4065
G00 Z0.0935
M5 M9
M30

Post by **MecSoft Support** » Wed Mar 04, 2009 6:16 pm

Jack,

R0.1 indicates the Retract plane for drill cycles.
To add G64 to the post processor, select Setup Tab in RhinoCAM Browser and click Post . This opens the Set Post Options dialog.
Set Current Processor to Mach3-Inch and click Edit.
Select the Start/End Tab. Under Program Start up code add G64 at the end of the 2nd line.

Before
[SEQ_PRECHAR][SEQNUM][DELIMITER][OUTPUT_UNITS_CODE]

After
[SEQ_PRECHAR][SEQNUM][DELIMITER][OUTPUT_UNITS_CODE]G64

Save the post processor and exit the post processor generator.

freshwatermodels · Post by **freshwatermodels** » Wed Mar 04, 2009 7:08 pm

Yes, adding the G64 can be done manually but I would like to get correct code from the post not from editing. The first version posted code that didn't need to be edited.

Jack

Post by **MecSoft Support** » Thu Mar 05, 2009 11:10 am

Jack,

Yes, adding the G64 can be done manually but I would like to get correct code from the post not from editing.

You don't have to edit the code. You edit the Post using the Post-processor generator and your code will have the G64 every time you post after you do this.

freshwatermodels · Post by **freshwatermodels** » Wed Mar 11, 2009 10:15 am

I tried inserting G64 but it didn't help. V1 of Rhinocam worked so well.

Why did V1 work so well and now V2 doesn't?

Guess I'm adrift between two software companies.

Jack

Hirudin · Post by **Hirudin** » Wed Mar 11, 2009 11:56 am

There is an option in Mach3 where you have to choose either "Exact Step" or "Constant Velocity" (AKA "CV"). It's near the middle/top of the Config -> General Config window.

If I were you I'd check what it's set to now and change it to the other one and see what happens.

Also, I see you're using G81 "Standard Drill" cycles. I just got done troubleshooting a problem with these so I figured I'd pass my fix along...

I recently made a part that needed to be drilled first. I created the MOps in RhinoCAM and ran the post processor. I figured I'd give the G-Code a dry run before actually putting the part in. It's a good thing I did because it was trying to plunge at 26 IPM (which is way too high for my machine (a Taig mill)).
After messing with the post processor quite a bit (I'm a big newb) I realized that the feed rate was not being set so the Mach3 would just use whatever it was set to last.

Here's what I did to fix the problem...
The settings for drill operations seem to be in the "Cycles" tab of the Post-Processor Generator edit window. The one for "G81" is labeled "Standard Drill".

I added...
[DELIMITER][FEEDRATE_CODE][PLUNGE_FEED]
to the end of what was already there.

So I changed it from...
[SEQ_PRECHAR][SEQNUM][DELIMITER][G_CODE][DELIMITER]X[NEXT_NONMDL_X][DELIMITER]Y[NEXT_NONMDL_Y][DELIMITER]Z[CYCL_Z-DEPTH][DELIMITER]R[CYCL_Z+CLEAR]

To...
[SEQ_PRECHAR][SEQNUM][DELIMITER][G_CODE][DELIMITER]X[NEXT_NONMDL_X][DELIMITER]Y[NEXT_NONMDL_Y][DELIMITER]Z[CYCL_Z-DEPTH][DELIMITER]R[CYCL_Z+CLEAR][DELIMITER][FEEDRATE_CODE][PLUNGE_FEED]

freshwatermodels · Post by **freshwatermodels** » Thu Mar 12, 2009 10:00 am

Problem solved by minor edit of the post with the help of Mecsoft tech support.

The tech was able to set up an on line meeting with me and actually SHOW me how to solve the problem on my screen! Wonderful support.

It's one thing to offer a great piece of software but it is when problems arise that one finds out just how good the company is.

THANKS,

Jack