First Post, First Project, & Some Questions

[dave benson]

HI Kelly

Great to see that you made progress.

If I set the machine origin at the top level of the machine tree, is it necessary to do so in each
part or can the lower level setting remain as default NaN? If they are different, which one takes precedent

If you place some numbers in there, and click back into the cb screen a red cross
should appear (you can move it anywhere including 0,0,0 ).

Is there a way to remove Machine Hold? When I get alarms, I can usually just use $X or one of the reset buttons to clear an alarm but I have to disconnect and sometimes reboot the controller to release a hold and regain the ability to issue commands.

If your talking about GRBLMachine then right click on the alarm and select
Alarm reset.

Kelley number 3 is a tin of worms really, because I'm using the Laser and the Grinder with a
win10 laptop  (both in the shop) ,I use a high quality cable 150 mm, and longer = worse.
I also disable the internet and do not use the laptop for anything else.
Set it not to go to sleep.
Some of the lased images from the laser thread took 12 hours or more and the
code ran through fine.

One thing, when working with GRBL on a microcontroller, it's tempting to when things
seem stuck to pull the usb cable out to reset the controller, sometimes you have to, but beware
that you can brick the (Windows)com port and have to restart windows to get it back.
If you have to Hard set the controller then give windows some time to register what happened.
On my old laptop I give it about 20 to 30 seconds before pluging the controller back in and this
has worked ok for me.

One thing more , when simulating the file, I was focused on the PP directives and not the mops, The only thing
I saw that stood out  was the sea of red in the sim, this means lot's of G0's at the clearance plane and the less
the better for efficiency sake.
Sometimes you have no choice, sometimes you can chop the geometry into smaller regions
enabling more (actual cutting timewise) efficient tool pathing.
I've have a look later tonight .

I would have suggested that you re-flash the firmware with GRBL Ver1.1 or maybe my 5Axis version of GRBL, But the manufacturer may have
adjusted the firmware (to maybe re-assign pins)  to suit their particular build practices.
So I thought better of saying anything.

Dave

[Tool-n-Around]

If you place some numbers in there, and click back into the cb screen a red cross should appear (you can move it anywhere including 0,0,0 )

Yes, I understand and have done so, but I only set the Machining Origin at the top level Machine folder. Machine origin also appears at each part level which I have left at default which is NaN. So since the files run fine I assume the top level governs unless a different Machine Origin is set at the part level, but not really sure why one would want to do so.

Kelley number 3 is a tin of worms....

I'll take your advice on that. I originally thought it was EMI issue because I would set my lap top on the CNC machine waste board and the touch pad would then become totally inoperable.......but it was of course also tethered to the controller by the USB cable, and it now appears that is really the source of the problem.

I do have a dedicated computer for the shop. I have cb installed on my everyday lap top. Since I was using UGS on the shop computer, I was just transferring gcode files on a thumb drive. Now that I have installed GRBL Machine plugin, I'm toting my every day lap top back and forth to the shop. I need to install cb on the shop computer but didn't want to maintain two instances while I'm in the steep learning phase.

I would have suggested that you re-flash the firmware with GRBL Ver1.1 or maybe my 5Axis version of GRBL, But the manufacturer may have adjusted the firmware (to maybe re-assign pins)  to suit their particular build practices. So I thought better of saying anything.

My computer administrative skills are also modest so probably wise to keep it simple for now, do some 2D machining, learn as I go and enjoy the benefits.

Best,
Kelly

[dave benson]

HI Kelly
To answer your first question

Yes, I understand and have done so, but I only set the Machining Origin at the top level Machine folder. Machine origin also appears at each part level which I have left at default which is NaN. So since the files run fine I assume the top level governs unless a different Machine Origin is set at the part level, but not really sure why one would want to do so.

I've posted this screen shot of a file that I use to cut ratchet wheel assemblies.
If you follow that file from start to finish in mop order, you get an assembly.
This is where your question comes in.
The stock for the components: 1 x 80 mm long x 40 mm dia 1045 bar.
1 x 100mm x 100mm x 6 mm  bar stock.

The 40 mm dia bar is held in a  4 jaw chuck on the mill for a few mops and then moved to a
four jaw on the lathe and back to the mill again, the flat stock is done in one set up in the 6 inch vice.

Anyway there are benefits from having different co-ordinates at the drawing
and part levels when doing more complex work involving having fixtures or maybe
a couple of vices and a 4th axis or like here a work holding chuck that has to be
indicated in then used then removed again. most people may never use this facility.
I have a few thoughts on your file, which I'll put in another post.
Hope that has not muddled the waters any further.

Dave

[dave benson]

Next....

I'm just starting to have a look at your file Perimeter Profile Part
The only thing I can see is using a starting leadin in the outside space mop
I've selected spiral leadin here.
This helps the witness mark that you can get with lightweight routers  when using no leadin.

Moving on up to Plenum and Throttle Bores.

The red I was seeing earlier was that port path had already machined away 0.25
of the Bore Pockets tool paths already and so set the Bore Pockets Stock Surface to
-0.125. 

I've simulated the file and it seems ok. If you set your Feeds and Speeds correctly you
should get a result.


In the sim pic of this original file that there is a sea of red moves, these are G0's meaning
that the machine is moving about the work piece without doing any cutting, for efficiency's sake
this is bad. I would before smashing the start button, make some test runs on a piece of
excess or left over stock material to get a feel for the feedrate that your machine is happy
with, before committing to the stock.

I made a new file that is more efficient Gcode wise (it does run and sim ok) but can't determine the
efficiency increase (by siming the two files and making a comparison) because I don't know what
maximum deep of cut and at what feed rate your machine is comfortably able to do.

I've kept the original (Plenum part) Port Path Mop so that you can do the comparison your self.
I've made a new Trochoidal pocket that uses the geometry split up in a different manner.

I've also re-arranged the Throttle bores part and mops so that there are very little unnecessary
moves.
At this point I have no way to safely determine what the Speeds and Feeds to put in the
Troch mops as the feeds and speeds in the Troch mops will be either faster or deeper or
some combination of both.

The Troc mops produce (peel milling) tool paths which are kind to your machine and cutter meaning
that in general you can make a faster cut by increasing the feedrate or depth of cut or both.
In a thread here somewhere I posted some pic's about the speed increase above the normal pockets
The cutting time reduction over a normal pocket varies over a wide range from a few percent to 60%
and very much depends on the shape of the geometry your cutting and your intended cutter size.

Our strategy's for setting the Troch mops would be different, I have a rigid milling machine with a low speed
head, you on the other hand have a lightweight router with a high speed head.

On my machine I increase the depth of cut and the cutting feedrate which yield some pretty good
results, but with your machine it would be best not increase the depth of cut but to increase the feedrate.

In the cases where the Troch mops can be effectively applied you'll be surprised at just how far you can push it.

I've done a lot of rabid cutting and pasting of mops in the file so even though it sims ok that
doesn't mean that I've not forgotten to set all the leadin's or starting points for example.

Once again I think that your file with those couple of tweaks will be fine if this is a once only job
things will be fine just get you speeds and feeds sorted.

For single simple once only files for one part  sometimes it's not worth it (the effort to optimise).
If you intend to make many of the same thing then the time spent on optimising the file is minuscule
compared to to how much time is saved machining.

Dave

[dave benson]

More pics

Dave

[dave benson]

Dang forgot the CB file.

One thing to mention is that the sim times are (for various reasons) a bit iffy, so the way I use it
is to run two files and by looking at the run time of the files compute how much one may be faster or slower percentage of run time.
To get a more accurate run time I run the code it through Mach3 sim which is has much closer
estimation of run time although not perfect either.

So I can say,this, one of these files will take roughly half as long to cut as the other.
The sim time in Mach3 was 1 hour and 32 minutes for the troc file and you still have to take this answer with a grain of salt
and is only an estimate. the original file simed at 2 hours 24 minutes.

There is one more set of optimisations that you can apply to the file (the last of the low hanging fruit)
where the load on the cutter can be taken into account (about 40-60 % improvement best case) zero improvement in the worst case.
As time permits I'll apply those as well to this posted file once you work out you maximum feedrate at maximum depth
that your machine is comfortably capable of,this is the figure the troc mops and the feedreate adjuster need and it must be reasonable accurate which you'll have to obtain by trial and error to some degree.
edit: to add another file with all troc mops
Dave

[Garyhlucas]

Simulations are always iffy because the programs know nothing about your machines ability to accelerate and decelerate. If your program has lots of long cuts the estimate will be better because the tool will reach programmed feed rate most of the time. With lots of short moves the machine may be programmed for 100ipm and actually only get up to 10ipm!

[Tool-n-Around]

Anyway there are benefits from having different co-ordinates at the drawing and part levels when doing more complex work involving having fixtures or maybe a couple of vices and a 4th axis or like here a work holding chuck that has to be indicated in then used then removed again. most people may never use this facility.

Thanks for the example. I understand.

...I'm just starting to have a look at your file Perimeter Profile Part. The only thing I can see is using a starting leadin in the outside space mop I've selected spiral leadin here. This helps the witness mark that you can get with lightweight routers  when using no leadin.

Was wondering about the lead in. So far I’ve only been cutting foam so not much of a challenge to even the little router or rattle the router bit. The phenolic composite for the spacer is supposed to be the most free machining variety but is quite a bit harder than hard wood. The only other place I might use a lead in for the same reason are the bores. When is lead out beneficial?

The red I was seeing earlier was that port path had already machined away 0.25 of the Bore Pockets tool paths already and so set the Bore Pockets Stock Surface to -0.125........In the sim pic of this original file that there is a sea of red moves, these are G0's meaning that the machine is moving about the work piece without doing any cutting, for efficiency's sake this is bad. I would before smashing the start button, make some test runs on a piece of excess or left over stock material to get a feel for the feedrate that your machine is happy with, before committing to the stock.

This was my first cb part and I was having difficulty trimming at the intersection of the bores and port path, so I merged them and cut them altogether and then had to go back and machine the remaining 1/8” of bore depth through. The stock thickness in the file says 1” but the actual part is only 3/8” thick. I had turned off all the cb optimization because I wanted to see the ops in order while I was getting errors, and also because I wanted to insure the perimeter was cut last and the guide slots after the port path.

I made a new file that is more efficient Gcode.....

Thank you very much for those. I downloaded them and took a quick look in cb. Looks like it doesn’t recognize the MOP Trochopock (unknown MOP Type) and missing some styles ‘Aluminum Drill and Mill” and ‘FeedRateAdjuster’, and also Tool Index (32) not found. I will look them over more closely a little later. I know I’ve read about tool paths for stock removal but couldn’t find that section on first glance.

One thing to mention is that the sim times are (for various reasons) a bit iffy, ……..The sim time in Mach3 was 1 hour and 32 minutes for the troc file and you still have to take this answer with a grain of salt and is only an estimate. the original file simed at 2 hours 24 minutes.

Ya-know, when I did the air cut, I don’t think it was anywhere near that long. 30-45 minutes, but, I backed the feedrates down from 120in/min to 60 in/min and cant remember if that was before or after the air cut.

As time permits I'll apply those as well to this posted file once you work out you maximum feedrate at maximum depth that your machine is comfortably capable of, this is the figure the troc mops and the feedreate adjuster need and it must be reasonable accurate which you'll have to obtain by trial and error to some degree.

I don’t have any experience with this little router. All my other router motors on my pin router are 3.5HP. Also, not much experience with the phenolic composite, so will be conservative. This a one-time part (though there may be other similar parts) unless I scrap it, so even though optimization isn’t that critical, it’s still good to learn early and on a familiar part because it will become a factor, and 50% reduction in run time isn’t a trivial gain, especially when I get to more complex parts.

I’ve been doing a lot of fine tuning to my hardware, software maintenance, downloading and playing with some plug ins, and just generally tidying things up. I also order stock and some parts. Hopefully I’ll complete all that the remainder of the weekend and get cutting. Thanks for all your help Dave. It is sincerely appreciated.

Best,
Kelly

[dave benson]

HI Kelly

Was wondering about the lead in. So far I’ve only been cutting foam so not much of a challenge to even the little router or rattle the router bit. The phenolic composite for the spacer is supposed to be the most free machining variety but is quite a bit harder than hard wood. The only other place I might use a lead in for the same reason are the bores. When is lead out beneficial?

I use leads (in and out's) quite a bit, leadin's more so though.

I use leadin's for two basic reasons:
When I'm cutting a 2D periphery of a shape or a slot, I use leadins to make the cut easier
for the endmill, rather than plunging down to the next depth increment and then start the next cut
the spiral leadin gives a gentle slope for the tool to enter the work.
There are times when stepping straight down can be beneficial, sometimes with a roughing
profile and an already pre-drilled hole to step down into so that the endmill is not doing
any drilling itself, for example if you have an endmill that is not center cutting.
 
I've posted a pic of port one with the Bore Pockets Finish Cut Deeper Mop selected and in the panel you can see the settings for it.(Tangent Leads)
This is the method I use when I want a nice clean surface on the hole.

I did go and have a look at the machining properties for phenolic's in general to ascertain what might be
a reasonable feed rate and depth of cut, endmill type ect,  and also (we barbarians call it Bakelite) now
I understand what the material is, just be careful with the plunge feedrates for the spiral mill are not to
aggressive. Here is a video of machining a phenolic spacer and they give there speeds and feeds, but
you can work the numbers back to suit your 4 flute endmill and your machine.
https://www.youtube.com/watch?v=6zRt_krMRgs

but the actual part is only 3/8” thick

If this component is a spacer and those port holes are through holes then  Then you may want to
consider using a spiral milling rougher Mop to cut out the bores rather than a pocket or even a Troch
pocket, as it will be much faster than either of them when applied to a through hole and would be my go to
mop if the hole was a through and not blind and I could also hold the stock so that the plug fell through onto
the table or vice jaws.

You seem to be steaming ahead Good Luck, when you get a result show us a pic.

Dave

[Tool-n-Around]

Cut my first parts today with success. Results here:

https://cambamcnc.com/forum/index.php?topic=9262.msg72543#msg72543

I decided to cut the air filter base and lid first because the foam stock is 50 cents and the Phenolic/Bakelite composite stock $50, so I figured a little experience under the belt would be wise......but this part is next!

Best,
Kelly

[Tool-n-Around]

Well, despite best efforts, I blew up a piece of phenolic stock. Posting this for feedback on whether I have diagnosed the problem correctly and to avoid recurrence.

I experimented on some small pieces with feed rates and found with a .25” 2-flute spiral bit, 30in/minute at .125” depth of cut to be about the max for this phenolic stock. Even that could produce a little chatter on the initial plunge but once it was cutting on side, it cut well. I even cut a sample piece of foam to try to de-risk the cut in phenolic stock.

I did rotate the part so I could set it up on the spoil board I had been working with. I cut the port passages with 2 passes at .1” and a final pass at .050” so the floor would have a decent finish. The roughing clearance cut was originally .015” and in what turned out to be poor judgement, I decided to increase the roughing clearance to .025”, and then I made a full depth cut (.25”) and .025” clean up on the profile.

Now, if I was a little more experienced, I may have thought oh, that  feature not being roughed out is going to be a problem on the next clean up pass and stopped the program, but I thought it was just a strange affect caused by optimization. It wasn’t.

Apparently, the problem was caused because the increase to .025” per side roughing clearance reduced the distance between the central boss and the plenum profile to just less than the .25” cutter diameter. I didn’t notice this on the foam trial piece but this appears to have caused the program not to cut the initial roughing passes between these features and then, when the program called for the full depth finish cut, the additional .050” clearance opened the clearance to greater than the cutter diameter and the program did at commanded and plowed through that area at full .25” depth and lost a bunch of steps (like over .25” worth) and then proceeded to plow through a number of other features at full depth until I got my hand on the stop button, but the part was scrap, but was otherwise looking perfect to that point. I went back and looked and this didn’t happen in simulations when the roughing clearance was .015” instead of .025”. So I measured the clearance in the model and sure enough it was .29x” t- .300”, so I closed the clearance down just enough for it to be fatal. -Sighhhh. At least nothing broke.

So I’ll have another go, but to avoid such problems in the future, how much clearance to bit diameter is enough as far as the program goes? I seen that a .25” cutter won’t drill a .25” hole, but will CB drive a .25” cutter through .25” openings? And if I watch each MOP in simulation and it cuts a path with narrow clearance, should I expect the same when run though the controller?

-Still learning. 

Best,
Kelly

[dave benson]

HI Kelly

Yeah you're summed things up pretty well.
just for some context.
I make components that are later to be used in assemblies out of mostly metal 1020 mild steel
fives series aluminium 1045 barstock. and some plastics like Delrin (POM) which is what your
motion system wheels are made out of.

In general I use  the spiral milling mop to cut plugs out or to make clearance for another yet to be performed operation.
This because the spiral milling op tends to produce holes that are not round,on size or
anywhere in the vicinity of where they are supposed to be. comparatively speaking.
The other thing is drilling (as an machining operation) is many times faster that spiral milling and
even with a tool change would still be faster than spiral milling on your job.

The bottom picture is a classic example of the high instantaneous loads you get in the corner
of the pocket, this happens when the tool radius is close to the endmill radius.

There are a few ways you can mitigate the problem:
1.. make the radius in the geometry larger  or use a smaller endmill   
2..Slow the feed rate down
3.. Use a Troc mop

With the Troc mops, once properly tuned and using the feedrate adjuster will  out perform
the standard pocket mop by a reduction in cutting time (at best) of 40 to 60 percent.
When applied poorly they can take longer.

I posted earlier a file with a comparison between standard and Troc mops but
could not set the feed rates, I'll use the value posted above for the safe max cutting speed
and then compare the cutting speeds of the two different methods.

The thing with the Troc mops is that they cannot be used universally  in replacement
of an ordinary pocket mop, only a subset of jobs will benefit from Troc mops.

IIRC your geometry  only allowed 30 percent reduction in cutting time.
If your going to cut foam and Phenolic's on a regular basis then look into endmills
for this purpose usually they have a higher helix (to get the chips to evacuate the cut better)
and 1 2 or 3 flutes but not four, I've used a HSS two flute slot drill (center cutting two flute endmil) for PP,PE,POM and some of that gummy big box store al to good effect.



Dave

[dave benson]

Hi Kelly

The first thing I did was move the geometry to the LLHC so the stock was
at 0,0,0 this was to get the sim in GRBLMachine to simulate  properly
as GRBLMachine is written with this convention in mind.(some of the jog section buttons)
are set up this way.
You don't have to do this I just wanted to see the sim work properly.
Later on I also entered the rapids that the manufacturer quoted so the sim will be a little
more accurate time wise. see pic.

I then set about comparing a Drill mop set up for a regular drilling operation G81
as compared to a drill mop set up as a spiral milling operation.

A problem appeared when I first generated the file, that being that the first
hole to be drilled was drilled 9 times and the other holes in the mop not at all.

I had to adjust the GRBLMachine PP to rectify this, when you get a moment
give your machine a test by, in a new file draw a few circles and apply a drilling
mop to them and see if you are getting the correct result.

One thing to know, is that for a spiral milling mop, the hole is cut at the cutting feedrate
and for a drilling mop the hole is cut with the plunge feedrate.

Comparing apples to apples the drilling method is twice as fast and more importantly
the holes will be placed as accurately as your machine can manage and will be round
enough for bolt clearance holes.

When I was at the manufacturer website I did look at the specs for positional and
milling accuracy  ---> positional accuracy 0.001   actual milling 0.004.
This is right for the motion system you have, but it's predicated on a new machine
with the correct cutter, cutting soft materials.

When I went to enter the new rapids into GRBLMachine things went sour and the
values I wrote into the X max feedrate ended up in the arc tolerance field in the
actual GRBL settings so I would be entering the values with "$value = some setting value"
from the console rather than just typing values into the GRBLMachine textbox's.

Anyway things are sorted out here now,drawing,GRBLMachine and the controller are
all playing nice together, however the other half has just  sashayed into the study
clasping the lid off the washing machine with a slightly distressed and quizzical look, so
I'm off to see how she managed it.
I'll continue on with the Plenum pocket mops after sorting that out.

Dave

[dave benson]

HI Kelly

I got some time to do the Plenum as a troc mop at 45 inches a minute the first file.
This would be a good starting point for Phenolic but too slow for foam.

One thing to know is that I've used no roughing clearance in this mop because
there is not enough room. so I would follow this Troc mop with a separate profile
mop at full depth.

The second file runs with a variable feed rate mode  60 inches a minute for the straight
a-ways and variable (according to cutter load)  from 60 to 25 inches a minute in the high load areas (the corners).

For the first file the feedrates are fairly conservative and with a little experimentation
you may be able go faster  testing on foam after a dry run would be the way to go.

The second file varies the feedrate according to load on the cutter, so the Idea
here is to do a dry run and then cut some foam. this gcode will make your controller
perform like a much fancier one (it will sound different) and if the file runs through and the cut surface is good and you believe that your machine can go faster than 60 in\min I'll provide one where the max feedrate is 90 in\min  but still keeping the cornering feedrate at 25-30 in\min.

This bit is optional
Once the maximum feedrate values for cutting foam and Phenolic are established
I'll fine tune the feedrate algorithm to suit your machine and supply a PP+PPT+Style and instructions to install them.

When you get some more Phenolic stock you'll have to determine the best feedrates
for it with the same method. this only has to be done once for each material.
edit to add: some versions of GRBL can not have a comment line over so many characters so I've provided one
with short comments just in case.
Dave

[Tool-n-Around]

Wow, thanks for that Dave. I wont be able to take it all in until tomorrow afternoon but am looking forward to it.

Best,
Kelly