Ezilathe, a useful aid to lathe programming.

Rengan77.
I just checked out your DXF for the chess pawn. Your profile is made up of generally individual polyline segments. This could be an issue, as the direction could be random, and possibly the odd gap in the profile. Much safer to join all segments required into 1 continuous polyline (No gaps, and all going the same way) as the Follow polyline functions do not correct direction.
Also split the big arc at 0 and 90 degrees to remove the unwanted part, and to allow Ezilathe to truncate the cut as required.
Parted it off for you as well. The head will still show a slight undercut from the tool radius and 11 deg lead angle. you would be better off with a sharp knife tool with no rad and 0 lead angle.

Hi Stutank,

Thank you for your reply. In regards to "face profiling" (sorry i am may not use the correct terminology), I am trying to see if i can profile the face of a round stock to make some sort of RC alloy wheel for my project.

Question 1
1. Attached is a picture of a sample wheel blank turned on some sort of cnc lathe (I guess). Since the face is of the stock is perpendicular to the axis of the lathe spindle, How and what strategy should i use in Ezilathe to achieve my goals if I were to use OD turning and the appropriate/recommended lathe turning tool ? - refer to wheel blank.jpg

Question 2
2. I have attached some photos describing the method of facing a round stock to obtain the profile as attached but this time using a lathe tool that is parallel to the lathe spindle axis; how do i model this tool and what process (i,e. OD turning etc) do i need to implement to achieve the required profile ? refer to Face Profiling example.png, OD facing R-L with tool perpendicular to lathe spindle axis.png and OD facing with tool parallel to lathe spindle axis.png

Question 3
Regarding with my chess pawn issue above with polyline, where i am getting so odd toolpaths, where no truncation appears. Is there any issue with the dex I sent ? Have you found a solution ? Something i am not doing correctly i guess.

thank you sir
best regards

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).
Another way to allow facing is to disregard (For tool checking) a final segment that ends at X0 (or slightly less for overlap i.e. X-0.5)
Any views on which is better.

Exe has been renamed, so avoid overwriting the existing version. just run Ezilathe1732.

rengan77.
Reviewed your Questions.
1) Wheel blank - Good job for trepanning, 1 trepanning tool (With or Without Radius) could complete the job. Your DXF could include other profiles on different Polylines and/or layers. These extra profiles can be initial stages in producing a form. For example trepan a groove around the mid point, sufficient to start a boring tool to do the outer half. The boss could then be OD Turned with a tool held as your Photo 4.

2) Face Profile example - Also can be done as a trepanning Job. I have adjusted boring to allow facing the end to X0 (refer post below). Works well, Boring is a neater option.

3) The Object of the polyline processes is to process as continuous profiles. Easier especially on complex profiles (> 100 segments), and considerably less error prone. Multi segment polylines will not have any gaps, and be 1 continuous direction.
Splitting a long radius that is "Re-entrant" helps in truncating the cut. (Check out my Chess Pawn.DXF from previous post)

Hi Stutank,

Thank you for your quick response to the Chess Pawn 1.dxf issue. Noted on the "continuous polyline".

I managed to regenerate the gcode OD turning profile as you advised. Attached are the gcode and the regenerated simulation at my site.

Noted on - "Also split the big arc at 0 and 90 degrees to remove the unwanted part, and to allow Ezilathe to truncate the cut as required.
Parted it off for you as well. The head will still show a slight undercut from the tool radius and 11 deg lead angle. you would be better off with a sharp knife tool with no rad and 0 lead angle."

Just wondering what is the best way to generate a dxf file from a 3D ?
Just to share with you how I generate the dxf with the following steps. I think maybe I am doing it in a not so efficient way ..haha

1.Create 3D model of chess pawn (I am using Solidworks CAD)
2.Save as dxf from Solidworks the side profile view.
3.Import dxf generated in solidworks into Vectric Aspire, where I define the origin (at the head of the chess pawn). I usually use vectric join vectors to join all vectors into a single vector
4.Export the newly generated dxf to overwrite the original one generated by solidworks.

Maybe you could share what is the best known method or practice to generate a dxf file ?

Best Regards
rengan

Your comment:-
1) Wheel blank - Good job for trepanning, 1 trepanning tool (With or Without Radius) could complete the job. Your DXF could include other profiles on different Polylines and/or layers. These extra profiles can be initial stages in producing a form. For example trepan a groove around the mid point, sufficient to start a boring tool to do the outer half. The boss could then be OD Turned with a tool held as your Photo 4.

My comment:-
I will feedback on this separately and soon after more experimentation.



Your comment:-
2) Face Profile example - Also can be done as a trepanning Job. I have adjusted boring to allow facing the end to X0 (refer post below). Works well, Boring is a neater option.

My comment :-
I simulated vith Ezilathe 1.7.3.1 and 1.7.3.2 and i obtained 2 sets of results and observation:-

1.7.3.1
ID boring Ezilathe 1.7.3.1 vector selection.png
ID boring Ezilathe 1.7.3.1 results.png
I have to have an initial hole diameter value (as expected) to allow for the boring bar to fit without crashing, the tool check warning is doing its job as expected.

1.7.3.2
ID boring Ezilathe 1.7.3.2 vector selection.png
ID boring Ezilathe 1.7.3.2 results.png
With initial hole diameter set to "0" the boring bar action definitely traverse outer diameter to X=0 as in my example (and vise versa).
Realistically i still have to bore out a hole to accomodate the boring bar since it will plunge into the material and will definitely hit the section of the tool that does not have the cutting surfaces.
I totally agree with you probably its is better to have the tool check enabled.
The trapening tool with "polyline movement" have a more "natural" facing movement where it digs into the face of the stock while moving radially. Please corect my observation if i am incorrect.
Ezilathe is already impressive as it is. My hats off to you Sir. Btw do you think it it necessary to have a separate Facing operation ?


Your comment:-
"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).
Another way to allow facing is to disregard (For tool checking) a final segment that ends at X0 (or slightly less for overlap i.e. X-0.5)
Any views on which is better.

My comment:-
I agree it should have the tool check enabled since the boring bar needs to have an initial hole to fit in. "Another way to allow facing is to disregard (For tool checking) a final segment that ends at X0 (or slightly less for overlap i.e. X-0.5)" - do you mean the tool check disregard the gcode segment ?
Will Ezilathe have a separate facing function in the future that can support the use of regular turning tool/boring bar that moves in a radial (first) and then axial movement ?



I have a question wrt the tools you model.I opened "Lathetdat" i noticed the numbers below.
Some are obvious but what do the other number mean ?
Are they specific to Ezilathe or they are standard defitions for lathe tools ?
How do I go about modeling a carving tool that is parallel to the lathe spindle axis similar to a boring bar ?

36,0,Carving Tool - 22 deg LH
3636,Carving Tool - 22 deg LH
0,0,0,0,0,0,1,
3,22,0.2,0.2,-0.2,0,5,0,0,0,0,0,0,

42,4,Test Trepan 2 wide 1 rad
4242,Test Trepan 2 wide 1 rad
1,0,0,0,0,0,1,
0,0,1,0,0,2,6,0,0,0,0,0,0,

30,3,Boring Tool - Small HSS
3030,Boring Tool - Small HSS
0,0,0,0,0,0,1,
20,68,0,0,0,4,10,0,0,0,0,0,0,

Hi Stutank

Just sharing my diy cnc lathe. I built from scratch. I got the old electrically faulty 7*14 lathe from friend and modded it to accept cnc stuff. Made some improvements to increase x travel and tighten up the mechanics for rigidity. I kept the original Z-axis (1.5 mm pitch screw) and X-axis (1 mm pitch screw) to cut some cost. Future I will upgrade to ball screws.

The controller is a parallel port based ST-V2, DM-556 stepper drivers, 4 channel relay module, additional optocoupler board for isolation and utilization 2 separate psu.

I am in the process of completion of a pwm (pin 17 of BOB) to analog + isolator board used to control the KBIC-120 (mine is a Chinese clone dc motor board HL-220AI) via potentiometer pins P1,P2 and P3. This will give mach3 ability to control the dc spindle motor. I will be adding a single pulse per rev opto-interrupter for the spindle index function. Just working out the physical mount. The function is tested and works well.

The pc is a recondition HP desktop PC with intel core I3 3rd gen. I added a PCIE X1 parallel port as the pc is fairly new and does not have built in parallel port. I am using windows 7 - 32 bit since it is recommended to work with mach3 for full features.

enjoy
rengan

Rengan77.

DXF from 3D
export as DXF or DWG from Solidworks - Good often do this myself.
Never thought of Aspire as a tool for cleaning up the exports from Solidworks. Anything similar to Autocad(2D) will do a good job if it supports polylines of any kind. I use Corel Cad Home and Student, for this job. As you don't need many features for this work, even a number of the Free 2D cad are up to the job. Many Simple parts, are just Drawn in 2D to begin with.

Any Boring tool job requires some kind of start (Drill or trepan, as large as practical) - Goes without saying. Disabling Checks are sometimes required (As in this case) but I always leave them on otherwise, but it still requires other correct data to be input to work (Such as Min Hole dia on the Tool definition (Which I do not want to Disable). At least Initial Hole Diameter = 0 means that you will put it back, to avoid deleting half the rough cuts generated. It might end up allowing the final end of the last segment only to go below "Initial Hole Diameter" and replacing the value required (No more "0", Assumes a faced end of hole).
Work is proceeding on Boring - Follow Polyline, and this could cover the question better.

Boring Tools - These are essentially just Turning Tools Turned through 90 Degrees (Dis-regarding Clearances of course), and this is reflected in the tool editor.
The shape of the tool defined here does not effect the G-code (Except where width etc are compensated in Grooving / Trepanning). Good tool definitions allow you to see in the simulator what the finished part will look like accurately (See clearance to shoulders in screw-cutting, and true finished size at angled faces or Arcs)

Tool editor data - Specific to Ezilathe - Don't change directly, Use the Editor.
Tool shape is very flexible in Ezilathe, so your Boring style carving tool could look like the one shown. Just play with it on screen, until you get what you want (Just move off the changed input to see it reflected in the graphic.

Hi Stutank,

Thank you for your reply and the explanation/information provided to model the turning tool in the same direction as the boring bar. I have added an identical spec tool "5252" as you have modeled and tried out some simulations myself. Attached are the results. I will try out the actual run of my cnc lathe very soon. Oh, btw noted of the excessive feeds and speeds you mentioned in my previous posts. I just set them higher than usual, for me to see the actual movements/results of the cnc lathe without waiting too long for its completion. I understand the feeds/speeds that I used is not suitable for actual machining, especially metals.

I have almost completed my cnc lathe conversion. I have a few more parts before I make some 'chips'. I will update with some photos of the parts made with Ezilathe once I have gotten it right. Anyway thank you for your time and effort to create and share a superb Ezilathe with the community. I am personally a fan of it. Its not easy to get started with GCODE programming. I personally learnt alot from Ezilathe due to its simulation capabilities and well commented lines. Most of the hobbyist don't have access to high end CAM (costs a bomb) and Ezilathe definitely fills this void. Cheers.

Stay Safe/Happy weekend

Best regards
rengan

Just uploaded an update to the "Ezilathe Beta Version" under Downloads/Others.
A number of changes to the latest version (V1.7.3.3)
The final end of the last selected segment of a boring job is not checked as suitable for the boring tool, to enable facing to centre.
(Allow Initial Dia for boring = 0 to disable all tool checks will be disabled next release unless problems occur)
Follow Polyline is now available in boring jobs. This allows more flexibility in laying out the cuts.
"Z Axis minimum" input is now enabled for All OD Turning modes. (Allows for material clearance beyond the end of the DXF - "For Parting off etc)

Exe has been renamed, so avoid overwriting the existing version. just run Ezilathe1733.

Rengan77
The latest Ezilathe is now available (See post below), it will allow you to face to center even with a quite solid boring bar. The end diameter of the last DXF segment is now not included in checking, but the rest are. This is not unreasonable position, that covers what is possible on the machine itself. A carefully profiled boring tool (such as T30 that I use) is the answer, but you may need to add some carefully chosen F or S words (i.e F20 or S3000 Low feed and High speed when cutting near to Center).
The Initial hole dia = 0 will be removed next release, as is not the answer (you end up with rough cuts starting at center, and not at the drill diameter) unless there is an issue (You can get creative with "Min Bore dia" under the tool definition, but I prefer to keep all these realistic).
Like to hear how you go on the lathe with all this.

Hi Stutank,

Thank you again, for Ezilathe V1.7.3.3. I will experiment and share my results very soon.

Cheers

rengan

Hi Stutank,

I am still experimenting with Ezilathe 1.7.3.3, and cannot get passed "Required Value Missing (White Edit Boxes). Honestly I have no idea where is the message pointing to. Could you help and pointing it out to me ? I tried changing from Cut Right To Left to Follow Polyline schemes but the result is the same. I think there is something I am not getting correctly to move forward.

Refer to :Ezilathe 1.7.3.3 ID Boring with fine boring tool 5252 to compare with Ezilathe 1.7.3.3 - pic1.png

I performed the same operation with Ezilathe 1.7.3.2 to establish some sort of baseline comparison where possible to see what i will get.

Refer to :Ezilathe 1.7.3.2 ID Boring with fine boring tool 5252 to establish baseline - pic1
Refer to :Ezilathe 1.7.3.2 ID Boring with fine boring tool 5252 to establish baseline - pic2

However I did get to test successfully Ezilathe 1.7.3.3 to understand how to use -----"Z Axis minimum" input is now enabled for All OD Turning modes. (Allows for material clearance beyond the end of the DXF - "For Parting off etc)". I tried to set "Z" Axis minimum -100 mm while my dxf ends at about -92 mm. I decided to test with a grooving tool 3333 just to see what I will obtain. I know there are grooving tool that can perform O.D turning and profiling too.

Refer to :Ezilathe 1.7.3.3 Grooving Tool min z-100 - pic1.png
Refer to :Ezilathe 1.7.3.3 Grooving Tool min z-100 - pic2.png

I also performed O.D turning with O.D Turning tool 3636 to compare with grooving tool, as expected the considerable gauging due to the back profile of the tool.

Refer to :Ezilathe 1.7.3.3 Turning Tool min z-100 - pic1.png
Refer to :Ezilathe 1.7.3.3 Turning Tool min z-100 - pic2.png

I will try out more in the coming days and will share the observations and results here.

Cheers
rengan

Rengan77
I seem to have Removed the "Initial hole dia = 0" in this release, and that is why you are being stopped with this message at this point.
However, the new (Final "X" not checked to allow for facing is in this release), so what you want to do is as possible in Ezilathe as it is on the Lathe itself as described below.

DXF start of last entity gives a 2mm Dia. All must fit in with this, so an initial hole diameter of 2MM max may be entered here.
Tool52 - Fine boring tool will need to fit a 2mm hole and still be able to retract in X, so on the tool record set "Min Bore Diameter" to a max of say 1.8mm, and the Clearance to 0.1mm (Min bore + 2 x clearance = 2mm). That will work in Ezilathe, and is quite possible on the lathe, if you take care with the tool.
The tool as shown would clearly have this shape covered (After drilling the 2mm hole of course), so all is well. Tool unlikely to fit far down a 2mm hole, so may require drilling out to say 10mm dia to just clear.

There are a number of things you can do to help on the machine i.e.
1) Rough bore all except the last 2 segments with a larger tool and delete the finish cut, before changing to Tool 52 for a final cut only of all.
2) Machine a second offset profile (From Cad) with a larger tool.


With some of these parts, not possible to get around them with 1 tool only, but Ezilathe does give a realistic view of what you will get (If your Tool list is accurate).

Hi Stutank

I managed to get it to work as you suggested. My reply as follows:-

1.Noted on the "Removed the "Initial hole dia = 0" in release 1,7.3.3". Is this going to be a feature in your possible next release ?

2. My last segment is < 2mm so if i selected the last segment with Initial Hole Diameter = 2 mm, Clearance 0.1 mm radially, Fine Boring Bar 5252 Min Bore Diameter = 1.8 mm will result in the error warning message "Initial Hole Diameter > Selected Entities - Finish Cut Depth at 1,67".

Refer to:- Ezilathe 1.7.3.3 ID Boring with fine boring tool 5252 pic 1 - Selected Last Segment.png

I think this is expected since the "micro"/ fine boring tool 5252 min diameter is 1.8. Noted on the "X retract" value of the boring bar movement. At the moment I don't have a micro boring bar with the min diameter of 1.8 mm and I don't think I will get one as I will have to drill a pilot hole of at least 2 mm. I know 2 mm drill bit is was too fragile and also has a very short reach. I agree with you in theory it will work, in actual scenario will work but may not be ideal and way and is too risky of breaking the drill bit.

Noted on your advice to use more practical 10 mm hole drilled to clear the more appropriate and economical larger boring bar.


3. Please note that I were to deselected last segment, I managed to get very close to your previous simulation result.

Refer to:-
Ezilathe 1.7.3.3 ID Boring with fine boring tool 5252 pic 2 - deselected last segment.png
Ezilathe 1.7.3.3 ID Boring with fine boring tool 5252 pic 2 - deselected last segment - result.png

I got a slightly odd last segment as compared to your result as my boring bar just machine all but the last segment.

Noted on the "Not all machining can be achieved with one tool"

I will definitely use your recommended machining strategy as you mentioned below :-

"There are a number of things you can do to help on the machine i.e.
1) Rough bore all except the last 2 segments with a larger tool and delete the finish cut, before changing to Tool 52 for a final cut only of all.
2) Machine a second offset profile (From Cad) with a larger tool."


4. I have a question regarding "Follow Polylines". I tried with existing tool 5252 Fine boring tool and selected only one segment to try out shown.

Refer to :-Ezilathe 1.7.3.3 ID Boring with fine boring tool 5252 pic 3 - Follow Polyline other segment automatically selected.png

It seems for me Ezilathe "automatically" selects all the segments I don't want. Any Idea why it does so ? I have attached the dxf for you to test out.

Cheers
rengan

1) Yes, But still an easy work around, refer tool min bore diameter.
2) Reduce "Tool Min Bore Dia" to get under DXF size (and X Retract, clearance). 2mm Drill should not be an issue, as quite robust. Keep spindle speed up, use Deep hole drill cycle (G83 refer favorites page) or drill out larger as far as possible. Less than 1mm dia drill is generally considered as getting "a bit small". I will try to improve this particular error message.
3) Odd profile is the Back of your Boring tool "Gouging" the work. You Still need to drill out, and face over center to get the result required. Your last segment noted at 1.67 dia, so adjust Min Hole dia to suit (say 1.4mm with 0.1 clearance). However somewhat pointless if you do not have tooling that matches, maybe look at a redesign.
4) If only 1 polyline available, it will select on screen complete, not just by segment. The dialog box is more versatile in selecting polylines, as it can select in reverse direction if required (but still complete polyline selected). Once selected, picking segments on screen will de-select them 1 by 1. The trick to a job like yours is 1 polyline for the bore, and 1 for the OD, or whatever is convenient. You can have multiple polyline as individual steps in the machining process. The reason that polylines select as a complete unit is that they can include many segments (My record is 98 segments).

Hi Stutank,

Sorry for the late reply. We are in COVID lockdown again :-(. I will look into your recommendations and feedback accordingly.

stay safe
rengan

We can see it is not good there at the moment, Hopefully improve soon for you. For the time being, better to keep your head down.
We are still in a good position here, and hoping to stay that way, so still be here when you 'resurface".

Hi Stutank,

We are completing week 1 of COVID lockdown which started on the 1/6/2021, The lock down will be until 14/6/2021 (hopefully). I am using the time to complete my cnc lathe enclosure. There are a few more items to complete. Attached are some photos of my progress. I will be making a hole in the lathe swarf tray and adding a "drawer" type swarf tray under the lathe to collect the swarf. The front panel will be a swinging type polycarbonate cover. All cables will route on the top cover for clean setup. I decided not to start making chips yet until i have the swarf collection completed. I like a clean setup as i live in an apartment and need all the chips to be contained within the "lathe box". I also completed the 1 pulse per rev tacho-wheel which i machined on my DIY cnc router. I need it for threading and can test the threading function in Ezilathe too.

Just sharing


Cheers stay safe
rengan

Hi stutank,

hope alll is well with you. I started with Ezilathe tool changes and noticed something.

If i were to select T3636 and select the segments on my dxf in which I want to perform the desired machining operation as i usually do as shown in figure "issue 1 - selected segments does not self clear - 1"

If i were to select a different tool T3434 the previous segments for T3636 does not get cleared. It will only get cleared if I were to change the direction of cut (or manually deselect the segment) as shown in "issue 1 - selected segments does not self clear - 2" & "issue 1 - selected segments does not self clear - 3".

The result is shown in figure "issue 1 - selected segments does not self clear - 4"

Is this intended or a bug ?

best regards
rengan