[V8Goose]

Hi & thanks for looking...

I'm bumbling my way through the lathe module of Dolphin (trial) trying to learn enough to decide if it is the right software for my meager needs.

I have imported a profile (looks like a fire extinguisher shape) to test and using the videos and help file have defined a tool and all looks ok (I guess) but the problem I have is it wants to cut the profile in a single pass.

My Sherline lathe can't cut the end radius (stock or billet is dia. 7.71mm acrylic) in a single pass and it seems that it wants to cut it like this regardless of the billet size I specify.

The tool is a 1/4" HSS right hand tool and I have defined the cut depth as 0.25mm. The final profile diameter is 7mm.

I don't understand how to tell Dolphin to take multiple light passes at the part, especially for the end radius...

Anyone know?

Many thanks in advance!

Goose

[andre-dolphin]

Hello,

Are you using the Profile Turn option ? I suspect you are, this is a finishing operation, and although you can specify a finish allownace you will need to produce a number of Profile Turn operations to machine from a billet.

You should use the Turn or Face command to "area clear" the billet, then use the Profile turn for finishing.

In the the Turn/Face command there a re settings for cut depth, finish allowance etc.

Also, on each on these dialogues click the Options Tab for more parameters, the one which catches a lot of people out is "Stay out of undercuts" this will prevent machining on undercut parts of the profile, it can be unchecked.


Hope this helps

Andre

[V8Goose]

Hi Andre...

Thanks for responding.

Yes that makes sense, I will try it out tonight.

Goose

[V8Goose]

That works, thanks Andre.

Would you mind explaining what an undercut is in lathe terms?

I'm a little stuck again also with outputting to a post processor for my Sherline lathe via EMC2.

Another thread says to use the M_EMC PP but you can't select an 'M' (I'm assuming mill) prefixed PP in the turn module and there isn't a T_EMC option.

I can't find one on the Dolphin PP page either...

I tried the Emco as suggested by someone else, but the resulting code is not the g-code I'm becoming familiar with.

Thanks for your help.

Goose

[Dolphin USA]

Try the attached post. It needs unzipped and compiled into the post processor module before using.

[V8Goose]

Perfect thank you.

I'm not familiar with the gcode format the PP outputs with the N-code line numbers and no spaces anywhere, but I can read it albeit much slower.

I will have to wait another day to see if EMC2 understands it hopefully much better than I

Cheers

Goose

[andre-dolphin]

Hello V8Goose.

Glad you are sorted with the post, there are also post processors on the Yahoo groups forum in the Posts folder.

As far as an undercut is concerned, it is basically like a groove but can be any shape.

ATB
Andre

[LeeWay]

The posts are also fairly easy to amend when needed. I had a lot of help from Hood at the Mach 3 forum. He helped me fine tune a post specific to my needs. Puts out exactly what I expect every time. You may learn a little about if from that thread.
Mach3Turn Offsets?

[V8Goose]

Andre...

Is the 'Stay out of undercuts' function there to allow a separate job to do a specific groove shape/style or is there another reason?

Thanks Leeway.

Cheers

[andre-dolphin]

That's basically it, leave re-entrant parts to be cut by another operation.

In some circumstances and with some profile shapes it can cause the system to report an error that the profile disappears when offsetting. This means that it can't calculate where the tool might retract to, as I say this only happens occasionally.

If you get this message uncheck the "Stay out of ....." box and re-run.

ATB
Andre

[V8Goose]

Understood, thanks.

[V8Goose]

So another step forward and another backwards as I try to get parts from my lathe/Dolphin combination

Any ideas on this one?

Last night I imported a .dxf profile into Dolphin and setup the lathe job. All looks good on screen and the resulting g-code too.

I ran the job and my lathe finally began doing what I expect except the result is perplexing!

I simply wanted to turn the diameter of my acrylic rod down a little and put a full radius on the end.

Pic 1: My profile in Dolphin.
Pic 2: An animation of the job shows the progressive 'bites' at the radius.
Pic 3: A finishing pass leaves a clean profile.
Pic 4: The result.

Sorry for the crappy pictures, I had to use my Blackberry.

Thanks for looking!

Goose

[andre-dolphin]

What does the graphics look like in MACH ?

If it looks like its turning the larger part of an arc, change the IJ mode under General config to ABS or INC - opposite of what its currently set to.

ATB
Andre

[LeeWay]

I wish I could help further with this. I get rounded edges when I call for them. It may be a function of your tool description or in Mach, I might suspect the IJ mode.
Definitely looks more like a bevel than an arc.

Opps. Posted right on top of you.
I think he is using EMC.

[andre-dolphin]

Sorry, just read previous posts and noticed you're using EMC. Is there a setting in EMC about arcs?

Do you have front toolpost ? it could be that your configuration requires the arc directions to be reversed.

ATB
Andre

[V8Goose]

Thanks guys, I appreciate your help!

Yes I'm using EMC2.

I don't know if/where the arc setting is, but I will find out tonight.

Yes my Sherline is a front tool post setup.

I'm off to research/understand arc directions now...

Cheers

Goose

[V8Goose]

Hi guys...

I'm continuing to troubleshoot this simple test profile and I've narrowed the issue down to the finishing pass.

I should mention the animation in Dolphin is exactly as expected however when I export the post pro. a line appears in EMC2 that causes the tool to cut the end of my stock into a cone instead of a light finishing pass around the radius.

The rough pass is correct on the mill.

The line that is causing the problem is:

N1135G01Z0.0
N1145G02X3.8Z-4.0R4.0 <-- This one
N1155G01Z-19.2

You can see that it moves the tool from Z0 to X3.8, Z-4 in a single pass thereby cutting the radius into a cone. I'm assuming the R4 is radius and that my issue is EMC's ability to acknowledge that radius and cut it instead of a straight line.

I have searched EMC2 for an arc direction setting to no avail but I may be missing it as it might be called something else. The documentation talks about G2 & G3 for normalizing arc output but the g-code from Dolphin is all N codes.

I can show you a list of the EMC settings if that will help.

As always, thank you for your help!

Goose

[V8Goose]

So for those interested in my frustrations... an update.

The problem below came down to two issues, 1: The output file had G17 in the pre-amble instead of G18 and 2: The finish pass line needed to be changed from a G2 to a G3 to change the arcs from a CW to CCW setting.

Every other arc in the .nc file used during the roughing pass works fine on G2, just the finishing pass needs changing. I can't get my head around that one.

Also I can't for the life of me get that radius on the end of my stock. The last 1mm or so is missed so I end up with a flat end on the stock (see pic).

For the Dolphin guys who are interested in solving this one, I have:

• Imported the profile from AutoCAD and used the DC software to draw a new profile.
• Set the datum and specified the spans & directions, saving the result as a .dra (I thought the problem might be the .dxf)
• Opened the new profile in CAM successfully.
• Defined my stock using the billet function.
• Defined my cutting tool and selected it.
• Cycle limits set to just larger than the profile, external, turn, finish z .1mm, finish x .1mm, cut depth .3mm, retract 3mm.
• Profile turn using profile name, X/Z finish 0.0, turn, forward, approach and runoff normal & 3mm

The animation looks perfect. The roughing pass leaves .1mm for the finishing pass and with the G3 correction in the code, the last pass cuts to the profile exactly. (see second pic)

I zero Z on the end of my stock and set the job in motion. I changed various settings and re-ran the job 8 times trying to resolve that last mm of radius to no avail.

Sure, these issues are bound to be my lack of knowledge with the software, settings or a combination of both but even my stubborness, tenacity & hours/weeks of trial and error are at their end.

My mill software is a joy to use, lathe software it seems is a holy grail.

Thanks for listening.

(insert emote of me shooting myself in the head)

[LeeWay]

I know it can be extremely frustrating. It was for me. It is just something you have to decide to accomplish. Stick with it. It will come.
Here is how I use it.

I use Turbcad and draw my parts in there. I draw half profiles for simple parts or full profiles and then split them in half and delete the top half.
The drawing on the screen reflects my finished part after part off. I make sure to join all the polylines.

Then I import directly into DCam. I never draw anything in DCad. No need to learn another CAD program.

Study that import screen and options. Minor changes here will effect the way the drawing is imported and shown.

I also generally use a profile from an older part that is close to the tools I will need on this one. Then I open that first, then import the new drawing.
This way if you have the same tool set and processes, you are ahead of the game.

If you don't need a particular process, you can turn them off individually in the left hand panel. Much like you can do with Layers in CAD.
If they are turned off, they will not show in the SIM or in the Post Processed G code. Careful with that.

When you describe your tools, you need to be incredibly accurate for good results. Same thing when setting your offsets in EMC.
I know Mach has a calibration aid in it to help with getting precise calibration out of each axis. Not sure about EMC, but regardless, the lathe needs to be calibrated extremely well.

Then of course, no flex at the tool is desirable. You start zeroing in on all that, and you will start to see faster more accurate results. Good luck with it and keep posting back. I'm pulling for ya.

[V8Goose]

Hi Leeway...

Thanks for your comments and encouragement. I had to walk away from Dolphin for a while to calm the rage.

I work in computer system design and I'm fully conversant with 5 of the industry standard softwares for draughting and modelling along with 10 years plus in engineering... I think my expectations are reasonable.

I too drew the 2d profile in another CAD program and imported it into DC's CAD package because I couldn't find a way to define the datum in the CAM module. As per the instructional video, I let Dolphin use the dxf to draw a new profile and pulled that through to the turning module, keeping it all 'in-house' so to speak.

I drew the end profile job from scratch this time, taking into consideration all you mentioned and carefully making settings and testing to see their results.

The last mm or so of the profile is missing again. I even tried cheating it by zeroing Z 5mm into the stock in both the software and on the lathe. No change.

What gets me is that on screen is correct, the animations perfect with regard to stock size and placement, the profile, cuts etc but the lathe doesn't finish the radius even though every other aspect is correct. (overall diameter, finish, part length etc).

Got to be the lathe, right?

So I scrapped this job... if I can't do this most basic operation then god help me when I need to do something complex...

Ok, so let's prove the lathe is good. I did a series of checks and it appears to be good, accurate to .009mm. Backlash and tool flex is minimal. Remember I'm cutting plastic as a test.

I decided to do a basic facing operation on the acrylic stock. I defined my stock in DC, defined the tool and selected the face operation. I set it up to start at Z0 and finish at Z-1 taking 0.2mm cuts.

Again the animation is perfect. I ran it on the lathe and guess what? Fail. I opened the g-code to find there is no Z movements in the operation *laughing* What a joke...

The lathe did as it was told and moved to Z0, X5 and then moved back and forth in the same spot per the code.

%
( Porgramme : O0100)
( PartNo : - face_1.cnc )
( Saturday, February 23, 2013 : 13:44:31 )
( Source File - face_1 : Post - T_EMC_FTurret_V11_30Oct12 )
N5G21
N15G0G18G40G49G80G90
( Turning tool )
N35T1M06
N45G54
N55G90G00G43Z0.0H0
N65S500M03
N75X5.0
N85X2.121
N95X5.0
N105X2.121
N115X5.0
N125X2.121
N135X5.0
N145M5
N155G00X20.0
N165G00Z20.0
N175M30
%

The animation on screen is <a href="http://www.goosesworld.com/dump/dc.mp4" target="blank">here.</a>

I've stuck with DC as a solution because it 'appears' to have all I need moving forward and it's in a price range I can afford but if I can't get even the simplest part from it in two solid weeks of (part time) effort I'm dropping it.

I have sent extremely complex parts to my mill via MeshCAM with so little effort it's almost a sin.

I need a drink or 5 :violin:

Cheers