G53 - Noted, I just treat as work offset Position (easy, no effect on output). However I note that effect on simulator shows a major crash possible. I will adjust simulator in the latest update to move directly to safeX / Z position to avoid this. Still no effect on Output G-code, but looks better. I hope you know you can replace G28 with G53 X0 Y0 (or Whatever) in the Lathe setup.
Your Drill bush - Rough cut #32 for left hand tool causes this as cut length is within the threshold distance off the final rough dimension (Cut length around 0.02mm). Probably better for me to ignore this cut, will check if possible. (You can Just delete the whole block). This is an unusual way to machine this, and by normal processes this would not happen. Plunging in and cutting with the backside of the LH tool is a bit risky, especially on a mini lathe. Refer the attachments for my take on this (Tool # and Depth of cut adjust to suit). Note that Your DXF cut can be extended adding a value in the "Z AXIS MIN" box , say -26 to do this. Then add radius with parting tool, at part off.
"G53 - Noted, I just treat as work offset Position (easy, no effect on output). However I note that effect on simulator shows a major crash possible. I will adjust simulator in the latest update to move directly to safeX / Z position to avoid this. Still no effect on Output G-code, but looks better. "
"I hope you know you can replace G28 with G53 X0 Y0 (or Whatever) in the Lathe setup." = Noted, I can do this, you did mention to me where to put in several posts ago.
Your Drill bush - Rough cut #32 for left hand tool causes this as cut length is within the threshold distance off the final rough dimension (Cut length around 0.02mm). Probably better for me to ignore this cut, will check if possible. (You can Just delete the whole block). This is an unusual way to machine this, and by normal processes this would not happen. Plunging in and cutting with the backside of the LH tool is a bit risky, especially on a mini lathe. Refer the attachments for my take on this (Tool # and Depth of cut adjust to suit). Note that Your DXF cut can be extended adding a value in the "Z AXIS MIN" box , say -26 to do this. Then add radius with parting tool, at part off.
I am not very sure where the box for "Z AXIS MIN" is located. Please refer to my photos. Have I got it right ?
I am unable to get the tool path to continue cutting past -23 mm in Z. Please take a look at my code and pictures. I cannot get the Z axis minimum to work.
Btw you used a grooving tool in an OD operation for the example you provided me earlier ?
I try to replicate it and it works just that that i get some sort of spike, what is my mistake ?
thanks
rengan
Last edited by rengan77; 05-16-2023 at 10:36 AM.
Reason: mistake
Rengan77
The green arrow points to the "Z" Axis Minimum input. Useful input here is a number less than the end of the last cut end. Your Z-23 to Z-26 for example. The cut will cut a parallel diameter from the end of your last cut to the Z dimension specified.
Your spike - Probably you have changed your tool 7 to have a 0.2mm radius (realistic for the MGMN200 tip). This is what you are seeing. Remove the tip radius to see the spike go (still be on the actual job in the lathe). I use a more traditional HSS blade rather than a carbide for parting-off with a sharp corner. Note Parting tool offset Left, so that Part length entered directly as the Z position and correct even if blade width not accurate.
Rengan77
Just uploaded V1.7.4.0 as a Beta Version. Please download.
Your Version 1.7.3.0 - this input was removed, but I found I couldn't live without it, so it was put back by V1.7.3.3.
Also G53 now works in Mach3 (Always did in Mach4).
You can always see what version is being used as it is the first line of any program produced
Thank you for the version 1.7.4.0. Thank you for posting it so quickly.
Noted on the items below. i will feedback after trying the latest version. Btw the previous official version is 1.7.3.3 ?
"Just uploaded V1.7.4.0 as a Beta Version. Please download.
Your Version 1.7.3.0 - this input was removed, but I found I couldn't live without it, so it was put back by V1.7.3.3.
Also G53 now works in Mach3 (Always did in Mach4).
You can always see what version is being used as it is the first line of any program produced"
I managed to simulate the drill bushing (without drill operations for the moment) It works like a charm.
Attachments are self explanatory based on the descriptive titles:-
1.Drill Bushing with ezilathe 1.7.4.0 17052023.txt
2,M5 G53 X0 Z0 off spinsle and return to home positions.png
3.Drill Bushing OD turn groove tool no radius -1.png
4.Drill Bushing OD turn groove tool no tool radius -2.png
5,Drill Bushing OD turn groove tool 0.2 mm tool radius -3.png
6.Retract Min Z dia.png
"Your spike - Probably you have changed your tool 7 to have a 0.2mm radius (realistic for the MGMN200 tip). This is what you are seeing. Remove the tip radius to see the spike go (still be on the actual job in the lathe). I use a more traditional HSS blade rather than a carbide for parting-off with a sharp corner. Note Parting tool offset Left, so that Part length entered directly as the Z position and correct even if blade width not accurate." >>>>>>> Noted and Understand your explanation. I did remove tip radius and the spike is less prominent as in the simulations.
"Also G53 now works in Mach3 (Always did in Mach4)." >>>>>>> Works well as in the simulations
"You can always see what version is being used as it is the first line of any program produced" >>>>>>> Noted as below
(EziLathe Version 1.7.4.0 Mach3 17/5/2023 8:25:48 PM)
(Dxf file = Drill Bit Turret Bush Bar = 25.3)
G18 G40 G49
G90 G94 G80
G21 (mm)
Sir, just wondering if you are planning to update the attached ezilathe manual Version 1.7 Jan 2020 to incorporate the latest changes ?
The improved Ezilathe surely is extra fun to work with. I tried to see if I can replicate a parting operation with a straight plunge/retract similar to the "misc canned cycles" parting operation. It was successful as in the attached program and picture
My machining strategy is based on what you recommended:-
1.spot drill and pack drill operation.
2.OD turning with 55 degree RH "SDJCR1010H07 - DCMT070204" with Z Axis Minimum @ -25 mm, from end of dxf of -23 mm.
3.OD turning with 2 mm grooving tool "MGEHR1010-2 - MGMN200" with no Z Axis Minimum = end of dxf of -23 mm for the radius segment only.
4.OD turning with 2 mm grooving tool "MGEHR1010-2 - MGMN200" with no Z Axis Minimum = end of dxf of -23 mm for the vertical segments all the way to X=0. It worked like a charm plunging/retract the grooving tool to X=0.
Rengan77
Glad you like it. If I may add a few comments :-
After the First Section with Tool 1, Under DXFSETUP change Stock Diameter to 16 (Finished head diameter) To Eliminate a lot of air cutting in the next 2 stages.
USE WITH CARE, NO CRASHES PLEASE.
The part-off is not very efficient (86 cuts). I use the parting off from the favorites, much quicker and produces better G-code. Having said that you could try settings as shown to Produce G-code as Listed. Currently Tool width compensation when you do not want it, You need to Delete Line arrowed. I will try to fix this for V1.8, but much better G-Code.
You can adjust Drill depth easily to end within the Part-off cut, leaving a good Face for the next component.
You can use from favorites the material set Z routines to setup for the next part.
As for PDF and help files, Some work still required, and will come out with V1.8 (Nearly there).
"After the First Section with Tool 1, Under DXFSETUP change Stock Diameter to 16 (Finished head diameter) To Eliminate a lot of air cutting in the next 2 stages.
USE WITH CARE, NO CRASHES PLEASE." >>>>> Understood and noted. I left adequate space (Z Axis minimum -25.5 mm) when OD turning with 55 degree RH "SDJCR1010H07 - DCMT070204" tool to allow space for grooving tool (Z Axis minimum = default dxf end -23) to come in at 16.5 mm X diameter. I gave some X clearance as well (might not be necessary). I am sure program will execute faster by having less "air cutting".
"The part-off is not very efficient (86 cuts). I use the parting off from the favorites, much quicker and produces better G-code." >>>>> I went with your recommendation using favorite parting operation from X26.3 to X0, Z-23 (end of the dxf)
"Currently Tool width compensation when you do not want it, You need to Delete Line arrowed. I will try to fix this for V1.8, but much better G-Code" >>>>> Noted on the tool width compensation. Hope to use V1.8 soon and test out. Btw why do you need tool width compensation ? Is it to allow some wiggling space and to minimize binding and load while using the grooving tool ?
"You can adjust Drill depth easily to end within the Part-off cut, leaving a good Face for the next component. You can use from favorites the material set Z routines to setup for the next part." >>>>> How do I use this ? Can you share the method/examples ?
Sir, I have attached the final "production" gcode generated "Drill Turret Bush 19052023.txt" and the simulation "Drill Turret Bush 19052023.png" for your reference.
Additionally, i would like to point out the corner details in the upper part of the simulation is not totally a mirror image of the lower half as in "Drill Turret Bush 19052023 2.png". I believe it is not critical but just to note here.
Sir, what is "Retract Min X dia " and how do you use it ?
What is "Work Axis, Range For Original Values Min/Max" ?
Referring to ezilathe manual 1.7 "Comments / Tips" below, if we were to use Gcode to handle initial facing cut, then obviously the next machining processes with be referencing to the original material origin Z=0 before the facing operation. This will cause in accuracy. How do we handle the process ? Do we faceoff and loosen the chuck and reposition the stock to the original Z=0 as I always do to provide a clean face to work with ? Is there any other way i can handle this, maybe ezilathe settings ?
"· Initial facing cuts - so many choices here!!! The default processing if the vertical end is selected is plunge into
center and face out to meet the od cut. You are better off to not select the end, and deal with the initial facing
cut manually in G code or on the lathe (or do not face the end, as often not required, or already done when
setting up the tooling)."
"Just uploaded an update to the "Ezilathe Beta Version" under Downloads/Others.
An additional to ID Boring function - Allow Initial Dia for boring = 0 to disable all tool checks.
The reason for this is to allow Facing to center if required.
The problem is that you can now put a large boing tool in a small hole (Not overly happy with this)."
For ID boring does the " Initial Dia for boring = 0" , i noticed it does not work in 1.7.4.0. Does this mean I cannot face to center anymore ?
The part-off from Favorites is the only 1 that I use.
Tool width compensation is required when cutting grooves that require "Z" movement so that groove is not cut to Width + Tool width.
Initial Facing cuts
Always when I start a new job, I face off the work and then set this face to Z zero.
No inaccuracy here.
All good unless Multiple Repeats Required (Avoids going out to manual operation, resetting the workpiece, facing, and resetting Z zero).
Try This from Favorites (Set bar to Z Zero, No facing required)
Material Set Z (Require Face/Turn Tool - Change X and Z)
T0505 (55 Deg Diamond LH Face/Turn)
G00 X14.0 Z0.0 %X set to contact the bar
M00 (SET MATERIAL OUT TO TOUCH TOOL - HIT CYCLE START)
G00 X18 Z1.0 %Retract to Clear
M04 S600
G04 P2.0 (seconds) %Wait for spindle to reach speed if Required
M08 (Flood Coolant On)
G00 X26.0 Z0.5
(Rough #1 R-L)
G00 X24.2
Or This if facing required (Collets pull back slightly on tightening or Face needs cleaning up)
Material Set Z & Face(Require Face/Turn Tool - Change X and Z)
T0505 (55 Deg Diamond LH Face/Turn)
G00 X14.0 Z0.5 %Z now allows for facing cut to Z Zero
M00 (SET MATERIAL OUT TO TOUCH TOOL - HIT CYCLE START)
G00 X26.0 Z1.0 %Set X to X Clear
M04 S600
G04 P2.0 (Seconds)
G00 Z0.0
G01 X-0.5 F20 %Face-off
G00 X26.0 Z1.0 %return to X,Z safe
(Rough #1 R-L)
G00 X24.2
Never happy with No Tool size control for boring, so removed. However to allow for facing the end of a bore, The final segment in a DXF selection is not now accounted for Tool size.
This now allows Facing to Zero, without removing all safeguards (You can "Lie" to the program about the tool size used if required). Cannot "Lie" to the lathe, Your Tool Width in "X" still needs to be < Radius of the hole at this point.
"Retract Min X Dia" - Used to prevent the Tool hitting the tailstock (Or usually Live center body) on the final retract to Home. Keep home close as possible to Z zero (Program Coords) make this less likely to be a problem (Especially when G53 Used). Just add a Diameter into the Box if required, Otherwise leave blank.
Simulation display - Other side is mirrored about X0. However limitations exist due to screen resolution, not to mention a tool path at 1 pixel wide on 1 side.
If you zoom in close (to the Cut side) you will sometimes see a deviation between the Black cut line and the green of the component (especially cutting at an angle or around a radius with a radiused tool form). This is an accurate representation of what you will get. The number beside "RES" in the status bar is the screen resolution you have, if you need to measure this deviation.
I am struggling again to make Ezilathe work. attached is a finial for a pen that I am turning.
I am using Follow Polyline. You can see the top line goes from left to right, that is what deals with the chipout. The remaining arc goes from right to left. If I run the arc all by itself, it works great. But as soon as I add the top line, instead of turning a finial, it turns a spear.
Any suggestions? I'm on version 1.7.3.0
Thanks,
Mike...
P.S. Here is the lathe setup, the yellow block is to be machined down to the diameter of the brass, so there is no LH plunging into the material! :-)
mikeschn
Been a while, I hope all good (except for this of course).
There seems to be an entity in your DXF that should not be processed. If you check the CAD COORDINATE FILE (Next page tab, next to GRAPHIC (BITMAP) ) you will see an entity #29 VIEWPORT [LINE] that seems to be added to the last LWPOLYLINE on layer 90 for some reason. I assume this should not be there (it is the line from 0,0 to 5.25,4.00) visible on screen off to the right. I just removed it from selection by clicking on it leaving what I hope is what you require.
I will look closely at the DXF, and see i can remove it (Let me know if it should be there, doesn't look like it).
The Jpg attached is what I get by removing this line (Keeping the 2 LWPOLYLINES, Entities 018 to 024 and 027 to 028)
Please note that you can process std lines / arcs and cut with followpoly. that final cut lett to right could just be a line from -0.875 to -0.625 and do the same (need to pick on screen however
Last edited by Stutank; 06-13-2023 at 01:07 AM.
Reason: addition
Is there going to be a way to delete lines that have been imported via dxf, that I don't want in Ezilathe? The "Delete Entity from Graphic" doesn't truly delete the line. It still shows up in the "Cad Coordinate File" tab.
Is there any plan to support ellipses or splines in the future?
How about changing the direction of individual lines and polylines? The "Select Complete Polyline By Number" icon isn't doing it for me...
Can you take another look at what I am doing? I am still getting a spearhead instead of a nice rounded shape... Check out these 2 pictures...
I've also included the new dxf file I started with as an attachment...
Answers to Questions
Is there going to be a way to delete lines that have been imported via dxf, that I don't want in Ezilathe?
No - The CAD Coordinates File is generated at loading, However I can Remove the "Read Only Property" if this helps.
In the Graphics window, the DXF LAYER DISPLAY check boxes can be used to show / hide by layer
The "Delete Entity from Graphic" doesn't truly delete the line. It still shows up in the "Cad Coordinate File" tab.
Correct - as intended, cannot see any purpose in removing from the Printout or the DXF File.
Is there any plan to support ellipses or splines in the future?
Not at this Time, Higher priorities. Until G-code directly supports them, the amount of processing is out of proportion with the benefits.
How about changing the direction of individual lines and polylines?
In Cut Right to Left and Left to Right, the Entities are followed in the required direction, no matter what direction they have in CAD. In Followpoly, the Direction is as Drawn, or Reversed via the Dialog. Where multiple polylines (or Single Lines / Arcs) are used, some may be picked reversed, or not reversed by using the dialog box multiple times. Note that any gaps in the Profile are "Jumped over" by rapid move at SafeX diameter. Note that Picking on screen will always Load in Drawn Direction, but De-selecting on screen a single entity from a Joined polyline will remove it and leave the rest of the polyline selected.
The "Select Complete Polyline By Number" icon isn't doing it for me...
Does it for Me. I can clearly see what I am picking here. Your latest works fine by pressing Select all button. Need more info if there is a problem.
Your Latest - 2 problems
1) Your CAD System is leaving unused data (42 Bulge) in the end point definition of LWPOLYLINES when it ends with an arc. You can see it's effect in the CAD Coords as 002 Segment [Arc] which should not exist. Never come across this before. Should be able to filter this out my end for V1.8. I resaved your file in my CAD, and only after exploding / and reproducing the polyline did this issue finally disappear.
2) I have an issue with Going to your Z-0.810, doing nothing and then going in rapid to the next X, and then to Z 0. Clearly I need to fix the start position when no cutting taking place. Only when it starts cutting at the Left to Right polyline does it the do the job as required. Will fix for V1.8.
At least you now have something to look forward to in V1.8.
Re: Ezilathe, a useful aid to lathe programming.
Reply with Quote
