Author Topic: Troch Mop Feed rate Profiler  (Read 8336 times)

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Troch Mop Feed rate Profiler
« on: November 01, 2018, 12:57:13 pm »
HI All

I'm going to stat a new thread here to iron out the details for the Feedrate Profiler for Troc Mops.

I post a few pic's detailing how to set up the new Styles and Modify the PP to suit your own needs.

All in all it's not to hard just make 3 new styles (Two Troc Profiles (Inside and outside) and one pocket).
Pop the PP in the PP folder along with the Profiler .exe.

There's a macro that you can set to a minimum Feedrate, the max Feedrate is set by your normal setting in the
Troch  MOP it'self.

I'll post a .nc file here for you to simulate or look at in the editor and if there's no Immediate problems picked up
I"ll post the PP and .exe .

What I've found in simulating is that Fully ratiometric feedrates tended to slow the actual cutting down to much  and
have gone to a bit of trouble to make sure that the Highest feedrate possible is achieved  during most of the cutting
and only proportional feedrates are applied where absolutely necessary.

Dave








Offline svse.cnc

  • Ewok
  • *
  • Posts: 9
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #1 on: November 01, 2018, 16:21:16 pm »
Hi Dave,

that looks really good. I have calculated the feedrates from your .nc-file. Do you multiply the feedrate with 2?
If i multiply my feedrates with 2, i get your results.

Is the reason to get feedrates nearly to the max feedrate, if the diameter is twice the tooldiameter?
I look forward to check your PP and the .exe on real aluminum parts.

BR Sven

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #2 on: November 01, 2018, 22:56:07 pm »
Hi Sven (hope that's your first name)

The first thing to say is that my hand coding skills are rubbish (I did do this a college, but they are distant memory along with my hair)
so be cautious (we have simulator plugin here for camotics) which on the whole works well and if you can you should use it before running the code on a job.
I've made the PP.exe only do Troch mops for the time being (just to simplify things for me when coding).
What I've found is that using a PP treatment of the code is much more limiting that using a plugin inside of CB, but in this case it's the only way to do it.
I've zip up my style lib along with (a PP.exe and a .dll that both go together in the post folder) which on my system go here :C:\ProgramData\CamBam plus 1.0
sometimes people have had trouble extracting plugins directly to this folder (windows permissions and sometimes the antivirus). there are threads here on how to get this going
but I've had no trouble extracting to my documents folder and copy and paste from there.
In the zip folder there are :

1... An xml file (the style lib)
2...The PP exe (itself).
3...A necessary .dll for complex vector math. this file is not included on a lot of usually older systems

This requires CB ver1
There is one more pic of my Machining folder (your's should look the same.
once you have copied the files to CB then you should save the file as a template
(this means that you don't have do the work all over again for a new project).

I'll post to more pic's of the Important things to note and hopefully you should be good to go.
Under normal circumstances to use the PP you should start a project from your template file (Troch FeedRate Template) as an example.
then select your style (my troch style) for example.

Remember you can set the minimum feedrate in the marco in the panel, I'm using metric so I've set this for me to suit  my machine, your's may be different.

It looks like a lot of instructions but it's one of those things that's harder to explain than do. Good luck

Dave.

Edit: OPP's made a mistake and posted the debug version (which I have to point at the file manually)
from VS studio so won't work.
I post a new zip (with a test CB file as well) so you can see how it's setup.
I would replace all the files in the folders with the fresh set.

I'm off to machine some 1018 HRS 4 mm deep with the new Troch pocket feedrates right now
and will report back when finished
Dave
« Last Edit: November 02, 2018, 06:55:15 am by dave benson »

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #3 on: November 02, 2018, 09:25:50 am »

Well that went better than I expected, just looking at the file I was worried that the feedrates in the corners of the job were a little too aggressive but the mill and tool seemed fine.
One thing I noticed was that the G1's ran at the last posted feedrate for the G2 and G3's so I've fixed that and will do some more simulating before posting the next update.
I also noticed that the profile mops were getting done as well, if they were in the same part as the Troch mop's
and have fixed that as well.
If I don't see any more errors in the Troch mops I may make the PP do all the mops.(small steps first).

The part in the pic is 1018 HRS, I'd already cut the pocket with Troch mop to a depth of 3 mm some time ago, and so indicated the part in and cut it to a depth of 4 mm @1mm  increment at 250 mm/mm (50 mm/m faster) that originally cut the first time.

Dave
 

Offline svse.cnc

  • Ewok
  • *
  • Posts: 9
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #4 on: November 02, 2018, 11:39:44 am »
Hi Dave, yes its my first name  ;D

i have installed everything and the pp is working!
But there is a little problem with the format i guess. See attached picture. The feedrate is set to 200mm/min (i'm using mm, too). The first G2 has the feedrate of 200.0 mm/min. The others have 2000,00 and there isn't any calculation of the feedrate.

Where do i set the min feedrate and the max feedrate? You sayed, "min feedrate in the macro in the panel".

BR Sven


Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #5 on: November 02, 2018, 14:18:54 pm »
Hi Sven
Glad you got it running, I've made quite a few changes and added a min setting to the PP which you pass through
I've zipped up the PP and .exe for you to try.
Hopefully the pic's will help, it's 1 am here and I'm not thinking straight now, and will post further explanations
in the morning.
Have fun, I've cut more pockets and they seem good.
Dave

Offline svse.cnc

  • Ewok
  • *
  • Posts: 9
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #6 on: November 02, 2018, 14:51:32 pm »
Hi Dave,

now i understand where to fill the min feedrate!  ::) Thanks

But the feedrate of F2000,00 is already there. What I'm wondering about is, why the F2000,00 is written with a comma instead of a dot? Everthing else in the gcode is written correct with dots.

Wish you a good night. Here it is 4pm now and i'm going home and into weekend now.

BR Sven

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #7 on: November 02, 2018, 22:32:53 pm »
HI Sven

Well the second coffee's kicked in, and I'm starting to wake up. ;D

At first I couldn't  think why the comma was there in your file and not mine, and you had "2000" not "200" but then remembered that CB has a number format  string (different countries have different formats using comma's to delimit the thousands ect) so I've posted what my number format looks like, so you can check with yours and make it's the same.
Once you have changed it remember to make the changes to your Template file, which you should use when starting
a new project using the PP. otherwise the changes you make wont stick and you will have to make the changes manually every time you want to use the Feed Rate Adjuster.
There are two places in the CB file where you can set the number format make sure they are both the same as mine.
If I get some time this Afternoon, I do some more checking of the other types of mops, to see if there are no problems adjusting feed rates in those mop's as well.

Dave


 

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #8 on: November 02, 2018, 23:47:55 pm »
One thing I might not have made clear, is that you can selectively choose which mops are adjusted and which ones are left alone by choosing another style other than the one's I provided.
for example the pic shows two drilling mops with different styles selected, one is processed and one not.
This way you can mix and match which mops in the same CB file are adjusted or not.
Dave
 

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #9 on: November 04, 2018, 00:12:19 am »
Here is the Latest version of the PP and exe.

I've changed the code to force an output without comma's (hopefully) as your os may override the CB one's.
I've also added a smoothing variable that can be set between 0.1 and 2, which let the Feed Rates stay high for longer
or sweep down to to a minimum feed rate quicker.
This is for working with different materials mostly, 0.1 holds the feed rates up for as long as possible, to 2 which is very sensitive to dia change and gives smoother feed rate transitions.

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #10 on: November 04, 2018, 00:17:43 am »
Here are three different versions of the same file with different settings for the smoothing variable.
you can open then up side by side in a notepad instance and compare them for reference.

If the comma drama is fixed, I think I'm done now as I've tried the PP out on quite a few of my files and it seems ok.
Happy CNC'ing
Dave

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 5115
  • Made in England
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #11 on: November 04, 2018, 17:01:18 pm »
Dave,

I'll bet you enjoyed that  :D good effort.
Filmed in Supermarionation

Offline svse.cnc

  • Ewok
  • *
  • Posts: 9
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #12 on: November 04, 2018, 18:12:50 pm »
Hi Dave,

the smoothing variable sounds really interesting. Unfortunately i have the same problem with the comma.
I will do some more tests tomorrow to manipulate my notebook. Hopefully to get it working.

BR Sven

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #13 on: November 04, 2018, 22:04:25 pm »
HI Eddy
Yeah it was a bit of fun, turned out that in trying to help Sven, I made something that is handy for me too.
It can be improved ( to run much faster ) but I"ll want Sven to be able to use it and report back before I do any more.
Here is a new version where I've had another go at getting rid of that pesky comma ::).
This should work for those living in the some of the EU countries.

Dave

Edit: one more thing before I forget, as the values in the Arg's line are parsed, make sure that there is a space between
each of the words and characters.
something like this: --->  "{$outfile}" minfeedrate = 25 smoothingvariable = 1 -->Works fine Note the spaces.
This wont work minfeedrate=25 smoothingvariable=1
« Last Edit: November 04, 2018, 22:13:08 pm by dave benson »

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1686
    • View Profile
Re: Troch Mop Feed rate Profiler
« Reply #14 on: November 05, 2018, 04:14:25 am »
I just had an inquiry from a friend where he spotted a 20 mm/m feedrate in a file he created, although he had set the min feed rate to 25 mm/m and asked "what gives" , well it turns out that he had also "in his file" set the spiral leadin rate to 20 mm/m so this overrides the minfeed rate setting in the PP. this correct behavior.

It turns out that I should have Measured twice and cut once with the pocket that I cut a few posts back, as I had to machine another 1  mm from the pocket.

And as the postie had dropped of some more 6 mm cutters today, I thought this might be an oppertunity to up the maximum  and minimum feed rates in the Troch pocket mop
and if I did the end mill a mischief than so be it.

I ran at 250 mm/m max and 100 mm/m minimum at 1 mm depth of cut and the pocket see pic below.

I mounted the work piece and fired up the compressor ( the Z axis mounted compressor works fine ) but I thought "just in case" as I expected a lot of chips.
I had to concentrate to keep the chips out of the pocket, but all went well and I believe that I could have made the Maximum Feed Rate 400 mm/m  but would keep the minimum feed rate at 200 mm/m (which was the feed rate I did the original pocket with, and this was to save the tool in the corners).
If the machine can cut at this speed (I don't know this as I've never cut at those speeds that deep)
and I can keep the chips cleared then the pocket  would take 6 minutes 46 seconds instead of the original 13 minutes 25 seconds.

Dave
« Last Edit: November 05, 2018, 06:11:06 am by dave benson »