setting up new post

I need some input on configuring my new post for the new system. I've selected the default "BC_4x_Mill.MillPst" post to modify to go with a 4 axis machine selected.

First, in the standard start of file (this will go for toolchanges and such also), the post had "n,rotary_angle" which outputs "just the number" with no A value. The controller, mach3 balks at this. I have changed it to the old output_rotary_angle and it works. Is this correct?

Also, looking at lines 440 and 441, I'm not sure what I need? In the old system, what would be output as a default in place of these settings? At this point I've set these 2 to 0, as I was trying to get rid of Mach3 errors on "inverse feeds". With the other settings, mach3 errors if a rotation angle does not contain a feedrate? Maybe I need to do some settings in my mach3?

I do have another question regarding the feedrates being output, but I will be meeting with my brother in a bit to be sure I know the right questions.

Thanks, I may use this thread a bit until I get situated.

Burr, Lets see if we can get you fixed up.

1. The post where the rotary_angle variable is from the initial release of the new update. If you modified that file in any way the the installer would not over write the file..causing you to keep the old copy. Replace the rotary_angle variable for output_rotary_angle, and also replace the second_rotary_angle with output_second_rotary_angle and this will be good to go.

2. Lets start with Q440. This question is defining the type of rotary axis you have. Most machines by default are going to use the more common mode 2. This is a mode called "Signed Continuous".

Let me quote the help system here for a minute:

440. What is the rotary output type?: Used to set how the rotary axis
angles need to be output for the machine.

0 = Absolute Position
1 = Signed Absolute (sign indicates direction to rotate)
2 = Signed Continuous

Explained:
0 - This mode is commonly found on indexing only machines. The positions around the rotary do not change and direction is controlled by the output of a separate Mcode to tell the controller what direction to rotate.

1 - This mode is commonly found on Fadal machines as well as others. The positions around the rotary do not change and the direction of rotation is controlled using +- signs. NOTE: you do not have to output the + if you do not need. There is a separate post line question for setting the sign for positive or negative rotation directions.

2. - This is the most common rotary positioning method from my experience. The rotary positions are like a linear scale...so 45 deg might position rotating 45 degrees in the CW direction..but -45 positions to a different location..being CCW 45 degrees. Using this method you can have rotary values that exceed 360 and will keep counting up as far as your machine limits can handle.


In Mach3 if you have the "Rollover" option turned off then your machine should run the rotary in mode 2 based on the list above

I will write another post to continue

AC

Looks like we have a developer/software engineer/tech/?? on here to help us with the new update.Thanx Alex


We'll keep an eye out for your pillow.Hopefully we will give you a chance to use it.

Next lets look at Q:441

This question is for setting the feedrate output mainly how it will affect output for rotary axes. Lets look at the reason 1st.

If you want to move 3 linear axes at the same time then inches per minute will work because each of those axes move in inches. A rotary axis is different. Based on how far the tip of the tool is from the center of rotation then the speed of the material will vary greatly. Rotary axes position in degrees and not inches...so only intelligent controllers can calculate this for you and allow a standard IPM type of programming.

The other solution to this is to use Degrees per minute...then the controller will calculate the XYZ axis to finish their moves at the same time as the rotary..this is very common for a single rotary but poses a big problem when you need to rotate two rotary axes at the same time, because you cannot have two different degree per minute feeds in one NC block.

This brings in Inverse Time Feed. This feed mode does sound odd and looks odd in the code as well. To keep it simple the system calculates the move of the tool on the surface..then based on your programmed feedrate will figure out how much time it will take to execute that move..then it outputs the inverse of that time value. This makes it much easier for the controller to know how fast to move each of the 5 axes to complete the motion that is needed by that NC block.

Now usually you only "Need" inverse time on lines of Gcode where there is 1 or more rotary axes moving. The system does however support additional modes.

Lets reference that help system again:
441. What is the feed type output for multiaxis?: Used to set how to
output feedrates for 5 axis machines this will directly affect the feed_rate
variable which is currently used for all feed rates.

0 = Unit Per Minute (programmed feedrate - IPM, MMPM, DPM)
1 = Inverse Time (for all motion)
2 = Inverse Time for only motion with rotary
3 = Inverse Time for 4 and? 5 axis simultaneous

Explained:
0-This mode outputs with Standard feeds UPM. For those who are only
running 3 axis this mode is fine. (so is mode 2...I'll explain)

1-This mode will output inverse time for all motion in a program. Even the
standard 3 axis moves will be output with inverse...This isn't too common
but support was added for those who need it.

2-This mode will switch back and forth between UPM for 3 axis (non rotary)
motion, and Inverse time (for motion that contains a rotary). This mode
works best for those who are using a rotary. This mode also will work for
those of you who have standard 3 axis machines as you will only get
inverse time output if the posting engine sees rotary motion..The new post
processor files default to this mode because it is the most universally
suited.

<edit> I forgot to add 3..lol
3-This mode will output the inverse time moves for motion that includes only 5 axis
motion..As it's name implies. All other motion will be output in UPM (unit per minute)
<edit>

For Mach3 setup with standard rotary mode 2 should work well for you..

So just a recap...running a standard rotary in Mach3 with the 360 rollover option turned off in mach..your settings are:

440: Set to 2 (Signed Continuous)
441: Set to 2 (Inverse Time on motion with rotary)


Hope this helps

AC

Please note that I am trying to provide helpful information that will assist with some of the issues you guys are having. Having said that I am human and can/may be prone to some blunders...please test carefully and determine that settings are correct for your machine configurations.

Hey Alex, I really appreciate the help.

So I set line 440 back to 2 and it seems to work without the error. The error is created by line 441 setting.

Here are 2 nc files that you can diff with the seeting at 0 or 2. The 2 setting for 441 produces a mach3 error of "F word missing with inverse time g1 moveline #" There is not much difference in the code except the output for "2 = Inverse Time for only motion with rotary" is producing G93 and G94 output (and some feedrates) where the "0 = Unit Per Minute (programmed feedrate - IPM, MMPM, DPM)" isnt.......

Is this a mach3 setting?

Also, regarding the Angle output, if you look at N86-88 you'll notice that 3 rotation values are put out together. The output should just be the full value to move it to? is there a reason for this incremented step in the rotation values throughout?

As a second item I'm looking at, is the safe and clearance plane output at the toolchange. You can see it in the 2 files I posted previously. In the start of program is set with regard to the top of part that exists. At the stop for the toolchange, it is absoluting to the .2 value set at the feature.

Thats this part of the end of the first tool

Code:

---

N1731 Z.1203
N1732 G00 Z.2
N1733 M09
N1734 M05
N1735 G91 G54 Y0. X0.
N1736 M01

---

Shouldnt this be a .1 value above the top of part?

If I manually edit the clearance plane at the machine setup level, it will output at the toolchange, but the initial value will include the top of part also, and be too high. Same goes with editing the rapid plane at the feature level.

Am I missing something at my toolchange position to read the value at stop properly?

Here is a test file with my post as i have it modified to this point.

What post processor are you using? Can you post it up here. It looks like your post is missing the variable "feed_mode" in some of your positioning blocks.

Reference BC_4x_Mill.MillPst.

Blocks 51, 53, 55, 56, 57, 153, 155, 156, 157

They all should have the "feed_mode" variable, and "feed_rate" variable.


A number of new blocks have been added to support the new features in V25. All this new stuff if going to be used will either have to be added to existing post processors...(it's not too bad) or rebuild the post using one of the new BC_xxx posts that get installed.

I will try to help with what I can.

AC

Alex, dont miss our cross post. I supplied a test file and the post I am configuring. I started with the default "BC_4x_Mill.MillPst"