I have never used Bobcad but cost was also a major factor for me and I got a really good deal from Dolphin and picked up the Mill Pro and the Lathe for the price of the Mill Pro only.  I have read several posts about BobCad that convinced me to stay away from it.  The lathe stuff I need to do is pretty basic.  I was even using pocketing code from Aspire that I manually edited to remove all the Z moves, but then I had to compensate for cutter plunge and retract, running the code in Mach to see what was happening. It was taking me from 3 - 8 hours of playing and testing to get a file that would work for what i needed, as opposed to a 20 minute task in Dolphin lathe (well at least once i get better at it)..   It all comes down to what works best for the particular person and the jobs at hand.
Pete

DICKEYBIRD,

Haven't used Doplhin lathe in a number of months here so starting to forget specifics.
Anyway.....

DOPLHIN TURNING POST PROCESSORS
Mach 3 - Radius mode:         T_mach3Rcss
Mach 3 - Diameter mode:      T_mach3DcssT

For version 10 and 11 I use the above post processors, but I mostly work in diameter mode and thus use
T_mach3DcssT and the code output for arc's are I k. I also have reversed arcs checked in my cofiguration.

Note the following changes for  version 11:

 As of Version 11 – a new section is required within all Lathe posts. This section must appear after the
Title section and must look like this :
VERSION:
FILEVERSION 11.0 TURNING
END

Dolphin worked for me for what I wanted to do. I plan on getting back into it in the near future.
Version 12? Well don't know if  I will spend money to upgrade. After a while you get tired of the upgrade crap.
I wish i had the money i spent on AutoCad over the years as i would be able to pay someone to do the drafting!

Till then,

RICH

If you look at your old posts you could tell if there used to be an issue or not.  What I found with V12 was that there would be a block starting with G00 (which tells Mach to use max rapid speed) then coordinates, the next line would also have X&Z coordinates but no prefix, so the machine would stay in the rapid feed mode.  The second line after the G00 is usually G01 plus coordinates.  At the end of this line there should be a 'F 5.0' or something similar to specify the required machining feed rate.  It is this Feed Rate command that does not show up in these instances, therefore Mach stays in max rapid speed for the duration of the entire process.

This sure makes for short machining times but really *********ty results, broken cutters etc, since you cant machine at max rapid speed......

So anyone that is using Dolphin Lathe V12 be cautious about this - and make sure you COMPLAIN to them about the screwed up post processor.  I tried all the post processors that were available - and they all do the same thing, they DO NOT change the feed rate.  So maybe this is an issue with V12, I have no idea, but it seems to me that it should be controlled by the post processor.

Perhaps Hood can shed some light on this?  Like I mentioned previously, Dolphin is now aware of this and it should be resolved soon - their post writer guy is on vacation or something...... I guess they don't have a backup programmer.... 

The V12 will now work with the V11 posts - at least on my machine, but they have been into my computer twice now and they have downloaded and installed several licence files, several new post processors and the like, so it is hard to tell what my machine is doing, at least it is workable for now.  the only way to test it would be to install the V12 demo software and try it out to see where it would be different from the V11, and also verify that the V11 and maybe even the V10 posts might work.  Rodney told me it would be ok to use an older post for the time being, so it should work for everyone, if the post produces proper code.

Pete


Pete

Thanks guys, it's good to see some Dolphin talk as there's not a lot of it around.  Unfortunately, life & other projects have kept me from using it much since the original post last year and I've forgotten most of what I learned.  I was able to successfully make a precisely turned knob for a friend's vintage cooking pot.  It had various blended radii & a couple tool changes and no crop circles or feed rate problems showed up so the T_mach3DcssT post works OK for my v10 anyway.

With the help of a programmer friend, we have figured a quick fix to the feed rate issue I have discussed above.  Once the g-code has been created in Dolphin Lathe, you can edit the code from the Edit menu using Notepad while still in the cam program.  All you need to do is to run a Find and Replace routine - Find G01 and replace ALL INSTANCES with G01 F3.0 - or whatever feed rate you want.  This of course is a global change but at least it shouldnt crash any tools on the plunge for you.  You can still edit any individual blocks you might need to change.

At least until the Dolphin post guy gets things fixed properly, this is a quick fix.  I'll let you know if/when the Lathe post is corrected, and also attach a copy for any that want it.

Pete