Editing your post processor

[Mark Bolton]

A question for everyone but hoping some of the veteran CNC'rs will chime in to ease my nerves.

I am beginning to edit my post processor for various operations. Simple edits, nothing drastic.

Here is my logic.

For instance when we are processing sheets I want the machine to park in a different location than the work home. I want it to return to the rear left corner of the machine to allow for unloading parts and loading the nest sheet. I also want the pins up when it lands in that position.

When Im processing solids I want a different set of actions, and so on.

So my logic is to edit the post and save a new post as a different file name like post_arcs_sheets, or post_arcs_solids, the name really doesnt matter just something that allows me to output to the post for the specific type of work. Its less of an issue of the post I guess and more so an issue of where the machine parks it self and what happnes at that point.

My manufacturer post has the machine coming to the work zero at the start of every operation after a tool change. This seems like a lot of wasted motion when it could just grab a new tool and start drilling 6" away. Also it parks at the work zero which leaves me manually moving the gantry out of the way and raising the pins.

I get paranoid making these changes and am hoping for some input on being on the right track, over thinking something that can be done more simply, and so on.

Thanks for any input.

[Brian Lamb]

I have edited and customized posts to better work the way I want the machine to... but I think you are talking about two slightly different things. Of course, this is somewhat dependent upon the software you are using, but Sheetcam is one I use, and it has "job options" that you can set that deal with parking positions, tool change positions, and add in any code you want before or after a tool change.

There are also different work positions, G54 is generally your 0,0 position of the sheet or work piece. then there is usually a G28 position that will take you back to the machine home position, sometimes this is the same as G53. You can always add another work coordinate, say to load/unload a sheet, G55 X0 Y0 will get you to that if you set it as such.

I guess I'm trying to say that there are about as many ways to do it as there are programmers, so it's kind of what works for you. It's easy to make changes and add code and run high off the part and double check to make sure things head the way you want them too.... you do have an E-STOP button don't you? Turn your rapids down and play...

[Gary Campbell]

Mark...
I may be able to add to what Brian says above, can you tell me what control software you are using and which design program's post you want to modify?

[James Biddle]

We've edited our WinCNC.ini file and some of the macros. I didn't like the position after finishing a file either. I also added a couple of intermediate steps for the warmup. My next foray will be to reduce the delay to get a spindle up to speed. We do like to walk through every one of these changes through tech support before implementing to avoid any unintended consequences.

[Mark Bolton]

Thanks guys. I figured there were several work arounds which was why I asked before I started tinkering.

We are Wincnc and Vcarve pro. Out putting with shopsabres post with arcs. I've written several macros that allow me to execute many of these handy options and work well. I have several of them programmed to macro buttons on the new xhc pendant but for instance when were are running a cabinet job my thought was to have the sheets post handle it so I don't have to even bother touching the pendant.

[Gary Campbell]

Mark..
Use one (or two) of the "P" positions and name it. Put it in the postP as "G53 P10" right after the G53 Z and spindle off commands. call that one "sheets" Make another with a different location for other uses. you select your park position by which postp you use.

[Mark Bolton]

My next foray will be to reduce the delay to get a spindle up to speed

James, This is one Im working on myself. Our current manufacturer post has the machine picking up a tool after tool change, and waiting for RPM's, then returning to X0Y0 to run the tool path. It would be great to have the spindle coming up on the way to X0Y0 (always enough travel for the spindle to reach speed) but then I can imagine if you cut out the return to X0Y0 and a toolpath happened to start 6" from the spindle location in the ATC.

Have you found a way to perhaps pick up the next tool, come up to speed as its moving to the start location, and if speed isnt there wait? Is that possible? My limited knowledge with Wincnc is its a line by line based operation. Execute one line, when complete the next, and the next. If thats the case it wouldnt seem possible to have the spindle coming up to speed while doing a traverse?

[Brian Lamb]

That I know of there is no "verify spindle speed" in g-code. You can always ad a dwell after your tool change, but it will most likely stop all movement while the dwell is being called before it moves. I do this on my CNC mill when I'm tapping holes. The speed on my machine can tend to randomly not get called, so I don't want my tap flying into the part at 3000 rpm instead of 1000, so I program a 2 or 3 second dwell so I have time to hit single block or the stop button before I crash the tap.

On a router I don't know how long the spindle takes to get up to speed, my mill gets there pretty much before I can move even a couple inches, so never much of a worry. You can put the M03 SXXXX on the same line as the first move, then it will be ramping up to speed on the move.

[Mark Bolton]

That I know of there is no "verify spindle speed" in g-code. You can always ad a dwell after your tool change, but it will most likely stop all movement while the dwell is being called before it moves. I do this on my CNC mill when I'm tapping holes. The speed on my machine can tend to randomly not get called, so I don't want my tap flying into the part at 3000 rpm instead of 1000, so I program a 2 or 3 second dwell so I have time to hit single block or the stop button before I crash the tap.

On a router I don't know how long the spindle takes to get up to speed, my mill gets there pretty much before I can move even a couple inches, so never much of a worry. You can put the M03 SXXXX on the same line as the first move, then it will be ramping up to speed on the move.

Yeah, The issue with our spindle at least is it is somewhat tool (inertial) dependent. A small too will be up to speed very quickly but a larger diameter tool less so. Talking about this issue is kind of like trying to wring water molecules out of a wet towel in that the time it takes to wait for the tool is not painful but in constantly thinking about speeding up and optimizing the process it becomes a point of interest.

Knowing the capacities and limitations of a 10Hp spindle compared to a 40Hp spindle in a Mazak is important lol.

I have played around with eliminating the return to X0Y0 in our post and there are the occasions where just by chance a tool path will start just inches away from the tool selected from the ATC and if there wasnt a dwell there (likely why the post always waits for spindle RPM before a move) it may make it to the work before its up in the power curve of the spindle and wouldnt recover.

[Brian Lamb]

Well, if your router spindle is 10hp, it shouldn't be taking too long to get to speed. As a question, the VFD driving the spindle, does it have a rather long ramp up to speed parameter? It's not uncommon to see a 3-5 second time to reach speed programmed in the VFD's, a lot of times because it's the stop ramp time also. But, you can set one to be different than the other, reset the spin up speed to 1 second and the stop leave at 5 seconds and that way you won't be heating things up so much to stop, but getting up to speed will be much faster.

That might be all you need to do to overcome the issue...

[Gary Campbell]

Mark...
You can do what you wish as long as the G0 X0Y0 is in the M3 macro, which I assume it is not. You can eliminate that command, I do in all of my posts. There is no reason to send a tool to any location, wasting time, after a tool change.

Look into the "M17" command in WinCNC. You will have to have an output in the VFD programmed to trigger when the "frequency reached" or similar and have that output connected to an input where motion is paused until the spindle is up to speed.

For my money, the "up to speed" and "spindle stopped" outputs that are integral to virtually all VFD's are mandatory in a properly working ATC system. Years of billable hours can be wasted by lazy programmers popping in a # second delay instead of doing it right.

This is most important when it comes to the tool release. IMHO the spindle stopped input MUST be checked prior to opening the drawbar.

In many VFD's there are up to 10 outputs that can be checked to either aid, dummy proof or speed up your machine. In many cases they are left unconnected and the WinCNC boards have open inputs.

[James Biddle]

Mark, we may have the same CNC. I agree with Brian that there isn't any verify spindle speed in g-code. There is a G4X3 command at the end of the pick up tool macro that dwells 3 seconds to allow the spindle to get up to speed that I think is too high. One second should be more than enough for our spindle given the distance from the dwell point to the cutting area, but I'll carefully observe at two first. I fully understand and support the manufacturer in shipping the tool that way and I try to carefully consider the possible ramifications before making any changes. To those who look at in making a 1 or 2 second change, it's not about any time savings, it's more about managing your machine to your expectations. That delay catches my eye as a possible issue, when it shouldn't.

[Gary Campbell]

James...
See above. There is a way to verify the speed is currently as set. it takes a couple wires, and 5 minutes to make it work

[Brian Lamb]

If what Gary says is available, an M17 that is checking for spindle speed, then use it. I just haven't seen that on many machines that don't have a spindle encoder on them for rigid tapping and exact spindle speed feedback.... but I'm coming from the CNC metalworking end of the world and don't know that much about the CNC router machines.

I don't know the WinCNC software, been dealing with Fanuc, Fadal, Milltronics... just recently started fooling with Centroid, haven't looked, maybe there software has something like that.

[Gary Campbell]

Brian, and Mark...
The "M17" command is simply a "wait for input" command. These are used often in ATC systems to monitor many system signals such as Tool in, drawbar position, VFD up to speed, VFD over current, Spindle overheat, VFD fault... the list goes on and on. They simply monitor inputs that are connected to peripheral devices. I am sure that "all the F's and G's" (my generic term for the alphabet full of industrial controllers) have them also.