Machsupport Forum
Mach Discussion => Mach Screens => Works in progress => Topic started by: RICH on November 27, 2010, 06:24:48 AM
-
PLease place any requests or post any wizards you may have that relate to the "THREE PAGE LATHE SCREEN" in this thread.
RICH
-
Wes,
I sent you the untested wizards for the lathe. Maybe just start with the 4 or 5 new ones.
RICH
-
I have taken the time to review and note those options below along with some + or - comments.
That provides a base to come from for constructive comments I will make in another reply.
My thinking around the wizard .....what additions to the therading wizard would make it more complete and if
possible would eliminate the minus and add the plus to have a single improved wizard if possible.
THREADING OPTIONS ( Note: that there are others but wil limit my comments )
1. G32 code
+allows for a single pass thread ( same as a G01 at a feedrate but provides for triggering of the thread cycle )
- not really a wizard or canned cycle
+required for picking up a thread (most users will probably never do it ) and can be used post a
threading operation to do a clean up / single pass / bring an oversized thread to tolerance if so desired
2.G76 CANNED CYCLE
+ it's a canned cycle that can be run from the MDI
- requires a " reference sheet" to use unless the user remembers the code
- multi thread dosn't work and hangs on the second G76 ( but then most users won't do or be able to do a satisfactory
multiple thread)
- settings in Mach Turn sets defaults for items if not specified in the G76 cycle ( so be carefull ) yet on the positive side
you can explore this and do some "wild" threads depending on the settings ie; like a acme thread with a single sharp v tool
if I recall correctly
3.SIMPLE THREADING WIZARD
+ Simple to use ( guess that it will be used by the bulk of users unless more advanced threads are desired)
- Requires a change to the M1076 macro for posted thread code to be in G32 or G76 posted format
+ Will calculate / check that you are not exceeding your max feedrate and acceleration ... and warn you...
I believe this is important and should always be run in the wizard.
4.QUICK THREADS
+ is more advanced, outside / multiple/work offsets / coolant & etc
- because it is more advanced, the user is faced with a more complex screen, BUT, the screen layout could be improved
to assist in inputing the numbers and the color of the text leaves something to be desired ( take this in the right way Scott
as i know how much effort it takes )
- the use of the minor diameter from the Thread Calculator will be incorrect for a sharp v thread ( should be .866x Pitch )
if one uses the calculator info... that is bad ...not your doing Scott, but very very important to note. Note that
the posted code from Quick Threads is correct based on a sharp v cutter.
+ provides for a for a caclulated spindle speed
5. MISCLEANOUS
G76_ threads ( in Mach directory )
- a calculator for showing comparison data for different type threading based on G76, Sandvik, Kenmetal
and not really a code generator. There are others from different manufactures which will give pathing based on their
specific tooling. Additionaly there is another wizard which does the above but the wizard is complex, never completed,
and should not be used.
RICH
-
Let the discussion begin....... :)
Suggest we just let a discussion take place, see how it all goes, and get more opinions on maybe what would be done ......if anything.
Maybe just stick to functionality as any screen changes ie; colors, text type, placement can be totally subjective and becomes a discussion in itself.
I'll start by "talking in circles" and one option at a time based on what i posted before.
1. G32 code
This would be a rather specialty kind of wizard to be added .
For picking up a thread a new screen would need to be done and VB code written to do what is required. BUT,
you have to ask how manny times a "year" it will be used if ever, yet....I don't know of a wizard or program
out there that provides for picking up a thread. Know the steps to do it....is it worth the effort?
The thought then goes to cleaning up or bringing an oversize thread to size, BUT, you can do that using your wizard as it is.
Yet, if your focused on the task a wizard could be handy.
RICH
-
Hi Rich,
Use the simple threading wizard for internal threads all the time. Define the start and end diameters correspondingly and it will do internal or external.
Dan
-
Daone/Rich,
Ok,
Rich: I would need a sequence of events and proceedures you need to do, to do a G32 and Pick-up-the-thread.
DaOne: other G codes via, pluign, the answer is not directly........ the G codes are done in machs interpreter, so to do it natively you would have to do it there.
if the interpreter saw in your G code whne you load it, a forien gcode, it will throw an error. Currently, custom "G codes" are done as custom M codes.
SCOTT
-
I would need a sequence of events and procedures you need to do, to do a G32 and Pick-up-the-thread.
Scott
I'll post something for the G32 first.
RICH
-
Rich, I haven't got them. How did you send?
-
Wes, I sent to your gmail address that you gave me
I'll check and see if the mail bounced......
RICH
-
Dan,
Here is what I got so far on the wizard you have requested. I am still finishing up on the code. Let me know what you think.
Wes
-
Wes, Sorry about that as it went to my draft folder. Just sent it a few minutes ago.
RICH
-
Dan,
Here is what I got so far on the wizard you have requested. I am still finishing up on the code. Let me know what you think.
Wes
Hi Wes,
Looks great! Exactly what I was meaning. Just a minor display note - the workpiece image is not symmetrical about the centre line.
Dan
-
Rich,
I got them. They look great so far. I like how they are commented in the G-code. I think this will help allot when we start compounding things to make programs. I have started writing the record functions and might need a little help from Scott. Still reading a few things. :)
-
Hi Wes,
Looks great! Exactly what I was meaning. Just a minor display note - the workpiece image is not symmetrical about the centre line.
Dan
I know its not perfect. Most of the image is from the standard wizards images. Looks like they were planning to make this but never did. Anyways I really hope that someone with more graphic skills than I can help on that part. I get frustrated quickly working with images. I do however use solidworks and can create the shapes and maybe even use real view to render them life like. Too many irons in the fire. :)
-
Wes,
A quick image. See attached.
Dan
-
DaOne,
I like how they are commented in the G-code.
Yep, forgot all about that, it's for dummies like me who only use them once in while and suggest that it is kept or added to in all the others. I can help with the bit maps.
Later,
RICH
-
Dan,
Looks Great. Any chance you can make it 275 x 253 pixels? Maybe even make the small one too for the wizard selector? They are 150 x 150 pixels.
Rich,
Yes I will be adding comments to all the code. It will really help in a long program.
-
Need a new one for the threading bmp, nothing fancy, just show a rod with thread on the end and a name. The current one was just a screen shot and looks like........
Later the tool paths, when appropriate, can be added to them.
Like the teamwork, just think what could get done if we had about ten people in here!
That said, i wil be traveling tomorrow, so out of pocket for a day.
RICH
-
G32 WIZARD
CURRRENT STATE OF THE MACHINE
Threading of the part is complete, spindle is turning / coolant is on , and X & Z axes are at some point along the axis. It is assumed that that current
modes ie: inches / exact stop and tool etc have not been changed. It's also assumed the user saved settings in the whatvever thread wizard was
used and has not closed the current thread file.
1. Spindle off
2. Reset / Estop/ the axes are disengaged for safety
MANUAL MEASUREMENT
The user will measure the thread, test with a thread gage, or try a nut or something to determine how much they want to remove from the oversize thread.
Most users don't even have a thread mic. I thought about having the wizard calculate what to do based on some measurements. It just opens up a can of
worms ( actual axis resolution, pitch dia basis, measurement averaging ) that is not worth having the wizard compute the correction. It's not only the as cut
diameter, but also lead , tool, and other things that can affect what the user ended up with. So KISS is going to be used such that only some spring
pass is generated based on whatever the user inputs.
INPUTS FOR THE WIZARD:
The X must be positioned and the same feedrate which was used in the threading wizard. Z start would usually be positive 3 to 5 x pitch from Z=0 of the piece, but,
who knows what someone used. There is a difference between say using Scotts, the Simple Threading, or a G76. So the question is where can the data
for inputs best come from ( other than manual input). Note that the G32 will not provide for pullout other than "0" setting for a chamfer at the end of the thread.
Scott, not knowing just what data you can or can't get may determine how the wizard is done ( or maybe shouldn't be done), thus some questions as follows:
? assume the current Z & X can be had from the DRO's
? can you extract data from the saved settings of the Simple Threading or your wizard.
? Is it possible to extract the last lines of code from a file and use them
Here is a list of data for the wizard: (> meaning data not input by the user if possible)
X> CURRENT LOCATION
X>END
Z>CURRENT LOCATION
F> FEEDRATE
X= USER INPUT FOR THREAD ADJUSTMENT
Z= USER INPUT ( MAYBE NEEDED IF CLEANING UP A MULTIPLE START THREAD / DON'T KNOW IF WE WANT TO GO THERE!)
F= USER INPUT ( i DON'T KNOW IF I WANT TO GET INTO THIS ONE.......EXPLAIN LATER)
N=USER INPUT FOR NUMBER OF PASSES
So the code the wizard provides will reposition the X & Z , an x move to a position, G32 move to thread the piece,
and a return after the threading to a position.
RICH
-
Ok Dan,
Give this a go... please be careful as it needs to be tested before you can rely on it. Also Mach does not display the stock correctly but the cuts look ok from the DROs. I would recommend cutting air a few times before using it to do any work.
-
Here are the correct size images.
Dan
-
Ok Dan,
Give this a go... please be careful as it needs to be tested before you can rely on it. Also Mach does not display the stock correctly but the cuts look ok from the DROs. I would recommend cutting air a few times before using it to do any work.
Wes,
All the other wizards work with "Reversed Arcs" checked. This one seems to require it be unchecked - otherwise the arcs look a mess. Anyway, it cuts a convex arc (like OD Arc 3). Also the Z Start and End (May be should be changed to Z Centre..) are swapped.
The gcode file puts out TyyyM6 for a tool change. The M6 needs to be omitted.
Dan
Dan
-
Dan, can you please post a screenshot and you code output? M6 is for a macro for people with auto tool changers.
-
Wes,
Attached are the screen shots and the corresponding Gcode.
The syntax for a tool change in Mach3 has been changed years ago, not requiring the M6. Tool changers don't require it neither. I have a tool changer and I only program Txxyy and it knows to refer to the M6Start macro.
Dan
-
Another note. I like my programs in feed per revolution, but I work a lot from the MDI as well where I need it in feed per minute, since often the spindle is off. Sometimes I forget to program G94 after the program and commanding a move in the MDI with a feed like F100 results in a rapid move. Can the Gcode have a G94 in the end?
It may not be convenient for people working in G95 from the MDI, but at worst they will get a very slow feed if they forget to do a G95 after the program. I think it is better than a rapid into the workpiece.
Dan
-
Dan, I am at a loss as to why your arcs look like this? I even tried your G-code on mine and it works great.
Must be something in the configuration.
Here is what it should look like...
-
Hmmm... Looks like some setting here. But then, just checked the other arc wizard and it shows a nice tool path with reversed arcs checked.
Will see if the incremental arcs may be affecting it, though it doesn't look to be the case here...
Dan
-
Dan, I would like the gcode output to work on things other than just mach 3. I don't think the M6 code hurts anything does it? Mach3s way of using gcode is rather limited and I am shooting for a balance. Adding G94 shouldn't be an issue since its the default setup on startup anyways. I will add it as soon as we get to the bottom of why your arcs look backwards.
-
Wes,
Yes, appears my arcs where set to absolute rather than incremental. Don't know how it was not affecting any of the other programs I was running. Changing it back to incremental fixed it :)
Most industrial lathes only use the T word for a tool change. This is how Fanuc works and this is why Mach3 was changed.
Dan
-
Dan, what version of mach are you using? I am wondering if you need a "I0." added in the mix. Most interpreters treat a missing "I" as a "I0." I wish I could find more documentation on how mach uses specific gcodes. Arcs always seam to give the most issues.
-
After checking some code... You are correct on the M6 on a lathe. I program mills quite a bit more than lathes and it is required on the mills. I will pull it out of the code. Give me a couple min and i will up a new version.
-
Here is the new file with those updates... It also fixes a couple issues I found in the last version. Let me know what you think.
-
Just tried to cut air. The tool would dive right into the stock, following the arc. Needs a few roughing passes based on the X start and final X. May be the rough passes should be G1 and only a few last passes would be G3.
The Z start and end are still swapped.
Also, the X start and X end don't seem to be defined correctly. X start should be the initial stock diameter. X end should be how deep you want the arc in the workpiece, i.e. not always would you want half a circle (this is what the current code keep doing).
Dan
-
I wish I could find more documentation on how mach uses specific gcodes.
You will find a lot of info relative to arcs on the lathe in the ARC Motion write up in Members Docs.
RICH
-
Just tried to cut air. The tool would dive right into the stock, following the arc. Needs a few roughing passes based on the X start and final X. May be the rough passes should be G1 and only a few last passes would be G3.
The Z start and end are still swapped.
Also, the X start and X end don't seem to be defined correctly. X start should be the initial stock diameter. X end should be how deep you want the arc in the workpiece, i.e. not always would you want half a circle (this is what the current code keep doing).
Dan
Something isn't right. The way the code works is this. It takes the X Start + the Radius of the arc + the clearance. This becomes the X start point for the Arc. It determines how many cuts to make based off your roughing depth and finish depth. It will cut to the X end and then rapid to the X start + clearance then to the Z start + clearance.
Are you cutting in diameter or radius mode?
-
Hi Wes,
I am in diameter. Are you saying that it will always do moves of half a circle? If so then the tool path was misleading - I saw it doing half circles and thought I will get the half circle in the part, but it appears to me now that part of the move will cut air. Will try to cut some material and see how it works.
Dan
-
Hi Wes,
I am in diameter. Are you saying that it will always do moves of half a circle? If so then the tool path was misleading - I saw it doing half circles and thought I will get the half circle in the part, but it appears to me now that part of the move will cut air. Will try to cut some material and see how it works.
Dan
Yes it cuts allot of air. In order to do it any other way would require allot more programming. Most of the wizards are very inefficient. The radius one I used cut mostly air as well until the final passes. The nice part is these are more less for quick one off parts not production runs so time doesn't matter much as long as the end result is the same. I made some chips with it today on a few test parts and it worked flawlessly.
-
Hi Wes,
Had a chance to cut some material today. The wizard doesn't work when in Diameter mode. The cutter plunged deep into the stock. Changed to Radius mode and changed the X values in the wizard accordingly and it worked fine.
The Z start and end are still swapped.
Dan
-
Please explain what you mean by "The Z start and end are still swapped." Are you talking about where the dros are located on the layout? They work fine for me in the calculations. I will take a look at diameter mode.
-
Dan I just tried this is Diameter mode and the code outputted appears fine. I would love to fix the issue if I could find one. Please post the code you outputted from the wizard while in diameter mode that is diving into the stock.
-
I have some additional wizards that you can use for your new screens. I posted these quite some time ago, feel free to include any of these you like.
http://www.machsupport.com/forum/index.php/topic,4206.0.html
Arnie
-
Sorry Wes, it was my bad about the Z values. They are fine.
It looks like in diameter mode the K word should be half the radius. See the code I posted in reply #23. Here are the last few lines:
(Finish Passes)
G1 X15 F0.05
G3 X15 Z-25 K-5
G0 Z-15
(Spring Pass)
G1 X15 F0.05
G3 X15 Z-25 K-5
G0 X16.5
G0 Z0.5
M5
M30
When is diameter mode, the last G3 move takes the cutter to the extreme X5, while the X end is defined as 10. Sorry for being unable to explain it better. Hope you follow me. Just change between the modes and run the code. You will see where the DROs go. Also load the OD Arc3 wizard and see how the arc movements are affected by changing the mode. I didn't try to understand the math behind it, but for some reason, in diameter mode the 'I' word adds up. In radius mode it's zero.
Dan
-
Dan, OD Arc3 wizard doesn't work the same as this as I keep the arc radius constant. I is not used. K = the radius of the arc. This will be the same in diameter mode as in radius mode. I will have some more time to take a look at this on the weekend. I have been quite busy lately. From what I see of the code I have outputted it looks correct. Make sure your in diameter mode when the code is posted. Also in diameter mode xstart and xend is the diameter. To check the code take a look at the "G3" line take the X value and subtract the radius value. The first line should be the clearance amount above the stock. I do see the clearance should be doubled and its not but that should still be ok as it wont hit the stock. I will fix that issue. Gonna have to test this on my lathe to see what is wrong or if it works like it should.
-
Thanks Wes. Although I am quite sure I was in diameter mode, I will check it again later.
Dan
-
Hi, I just found this thread and have downloaded the new wizards. I will give them a try soon. It is great to see some work being done on the lathe side of Mach3.
If you are taking feature requests for the existing wizards, it would be great to have a tool number field in all of the wizards that don't have one already.
The first couple of times that I used the OD groove wizard I managed to attempt a 10mm deep initial cut with my parting tool, with disastrous and fairly expensive results.
I subsequently worked out that I needed to edit the gcode output from the wizard and input the tool number ie: T103.
Anyway thanks for what you are doing.
Cheers
Dave
-
Dave,
Yes. I am going to add tool number, rpm/sfm,-css, fpm/fpr and coolant to all of the wizards. Please use my new wizards with caution as they haven't been tested enough by me to consider to be 100% safe. Dan was reporting some issues with diameter mode on the OD Arc3 wizard but I haven't had the time to test it yet.
Wes
-
That's good new about the tool numbers Wes, I tend to use everything with caution due to my limited CNC experience. I did read through the thread so far and saw Dan's issues, but I always use radius mode, so I may not see that one.
What did Dan mean by his issue with the Z start and end being swapped?
Cheers
Dave
-
The issue with zstart being swapped was never an issue. I think he was just looking at it wrong or something? I use radius mode as well and tested the wizard quite a few times in that mode. It worked flawlessly for me. One thing to be aware of. CSS and FPR don't work together. I had my lathe try to start cutting at what seamed like rapid speeds after a few passes. We have also noticed the FPR by itself isn't cutting correctly as well. Just a couple of the many bugs in mach 3 lathe. I am hoping Brian can work his magic someday and fix these issues.
-
The issue with zstart being swapped was never an issue. I think he was just looking at it wrong or something?
Correct. Was my mistake.
Haven't had a chance to mess with the OD Arc3 some more, but, as reported from the few tests I did, there was an issue in diameter mode.
Dan
-
Hi again, I hope you had a good Xmas, playing with the lathe again today, I accidentally ran a wizard generated gcode file without inputting a spindle speed... duh!
It would be great if all the wizards had a mandatory spindle speed field as well as tool numbers.
Cheers
Dave
-
Hey Rich (and who ever it was that did the 3 page lathe screen).
I did a screen set called "Practicle Lathe" http://www.machsupport.com/forum/index.php/topic,3653.10.html reply #14,
probably for the same reasons that the 3 page lathe guy did his. I think both screen sets have thier advantages and disadvantages.
If there is interest in "Merging" the two types of screen sets, taking the best of both, then I would be willing to help him, or he help me, or what ever to come out with a New hybrid lathe screen set.
(further, I would also be willing to do that screen set in an optional "Flash" version for lower CPU consumption/loading.).
Lathe is a VERY neglected end of mach3, I use a Lathe, but at the hobbiest level of skill. Having said that, for you guys who are lathe user GURU's, if you would tell me, WHAT and HOW you want the Wizards to do, I would be glad to make them, OR, help who ever make them in a joint effort that would help the community (of lathe users), at large.......
Scott
-
Scott,
A nice hybrid screen would be nice. I personaly can certainly go for that and yes they all can be merged for the best of the best.
How to go about recounciling users preferences to achieve that is another story. A way to do that would have a bunch of folks just sit down and plan it out.
Hood had a post on what a new generation lathe screen should look like / include, asked for suggestions, and there were a number of replies.
I can do a some leg work and have a a look at "all" the screens that have been done and compare as there are not that many.
I could put that into a file here for review to start things off if you wish.
I lost track of the other post on wizards . That's a different subject but should be planned for.
Your or anybody elses thoughts on the matter please reply?
RICH
-
For sure,
Lets consider not just a Hybrid Lathe screen, but an "Update" or extension to the current lathe wizards.
The heavy hitters (or at least prolific posters on lathe issues), seem to be:
Rich
Phil
Graham
Hood
(I am sure others but cant think of them off top of head).
I would be more than glad to contribut to the screen build, Wizard(s) build, what ever, and would be glad to incorportate:
a "Hybrid" Threading Wizard, in where, this ONE wizard would have a initial page in where the user could pick, simple or complex threading.
it would then jump him to that page, then the user could make choices from those pages. We could put together "ALL THE BEST" parts of the various
simple and complex threading stuff into the threading Wizard, that might include "Accurate" threading charts as HTML info screens, etc.....
Further, there are several guys like Graham who are walking "Yoda's" of G Code, that could probably submit VB code to do "Smart" Wizards for various operations.
So, if you or others have "Formula's" and/or fancy G code stuff that they would like to happen behind the seens, then submit it.
NOTE:
It would be good if one of the "Admins" could make a temporary thread called "The Lathe Project" with Special account priveleges.... in such anyone could edit a single post, i.e. I put a list of stuff and ideas up, then the next guy could EDIT my post to add more to it....... that way, you would have ONE single post that all who are interested could talk about this, and when all is said and done, then, lets make the screen and wizards........
Purhaps have another sub-thread for "The Screen" where we could put up a lathe screen, then some one else could take it down, and modify it, and repost it back up, in the SAME post, it would be like a community project file........ Same for the "Lathe Wizard Suite".
If this is NOT do-able due to the constraints of this, site, them if someone has some vacant website space or what ever, that we could put that "Link" in a post, then you could goto that site, pull down the current screen, wizards what ever...... work on them (anyone could who wanted to) Some kind of CVS system like Steve Murphy did for the Galil plugin..... as people add stuff, or fix stuff, it tracks the changes......
That way, the burden would not be on ONE or TWO guys....... there are MANY, MANY, MANY talented people on this site, that have made GREAT screens, and Wizards, or G code or Graphics(bit maps)........ etc........ everyone brings something to the table...
scott
-
I was playing with creating a conversational wizard for the lathe. Basically it would work like the newfangled one. You can create a full program by using the individual wizards to build the program. My biggest issue is figuring out how to add to and remove from the teach file. Maybe that is something Scott can help with? The G-code is the easy part for me since I use it everyday on the big toys.
-
yes, doing append to the file is not really an issue
scott
-
Maybe you could show me how its done? Basically I will have a universal setup page that sets up the machine, has a material database, units and so on... Then each wizard will be amended to the same file as they are "posted". Basically a type of record function. I would also like to make the ability to list the steps in your program and erase them if needed.
-
Good ideas guys. I agree on most of the things. While I am not a programmer and never built a screen, I will try to contribute as I can.
Dan
-
I would be more than happy to test things as well as to provide feedback and encouragement for this endeavour. I am not sure if I could contribute anything concrete, but you never know I am slowly learning.
Cheers
Dave
-
Scott,
I'm doing some searching on user Lathe screen preferences from user replies and the different screens done to date.
Hopefully Hood will find the thread containing those replies.
Then i will get into the wizards. For now......
There are three threading wizards done along with screens. A friend found a problem in the Simple Threading Wizard and we know the fix.
I need to review your complex one.
I have some new wizards that can be added to the turning wizards screen.
Will get the macros on drilling that can be turned into a wizard screen and if you want I'll write the logic on picking up a thread or fixing a thread and that can maybe be turned into something.
Later......,
RICH
-
Scott,
"The Lathe Project" with Special account priveleges.... in such anyone could edit a single post
Can't do that.
Suggest we just create a nice new thread "THE LATHE PROJECT - 2011" in Works in Progress. We can sanitize it as things develop....?
It would be dedicated to just the screen and let the wizards develop here.
Any other ideas...?
RICH
-
Done...
http://www.machsupport.com/forum/index.php/topic,17093
-
Rich or anyone else please help me locate the newest lathe wizards and their screens i have searched my brain numb
i understand they are all or most in beta and i would like to test them.
finding the complete setups in a zip is killing me lol
i'm interested in the 3 page lathe screen wizards very much and anything else
i can help test i use my hobby cnc lathe and mill every day
any wizards for mill would be nice also
thanks
attached is my work in progress pics I'm a serious mach3 user and would thank anyone for any help
-
the pics i sent are a model of the yulee sugar mill
thanks again
-
Steve,
Here is the link for info on the screen set which includes how to install it.
http://www.machsupport.com/forum/index.php/topic,13548.msg88932.html#msg88932
As far as the wizards used, they are the ones that come with Mach3.
BTW, nice project you have going there....,
RICH