I have recently got BobCAD Mill and Lathe and have been testing things out.
It is quite a learning curve, but that is true of all software when you are new to it.
 So far I have only tried Lathe but it is working well. There are a few issues, some of which I have sorted and some of which I haven’t.

The things I have sorted out are the post processor was posting quite a bit of junk and Mach would just error when loading the code.
Things that were wrong were I and K round the wrong way, so some arcs produced full circles instead of small arcs.
G97’s being called without a spindle speed,
G76 threading code had two X and Z calls  in it.
CSS surface speeds being called when they  shouldn’t have been.
CSS speeds were based on the rpm that had been entered so were way too fast anyway.
Tool list call in the wrong section so it made the first tool selected wrong.
No G95 being called
No G91.1 being called
Few others that I forget


Ok so got that sorted and it was posting good code with the exception that because I was in Dia mode the X Toolchange positions entered in BobCAD were being doubled. I have not managed to sort this yet  and not sure if I can. It can be solved by entering the toolchange value, in BobCAD, at half the dia you want but  would be much better if BobCAD didn’t double it in the first place.


Another issue I have is the machine setup in BobCAD will not stick to metric mode, I change from inch, click save then next time I go back in it is back to inch. This does not really seem to affect things too much, if indeed at all,  as you also  set the defaults in the CAD/CAM itself and the metric/inch will stay at whichever you choose there.

I took bad with the speed of toolpath generation, it was very slow compared to any other CAM I have used. I enquired about this and was informed it was because I was using CAM toolpath compensation and it was doing a lot of collision checking. I switched off CAM compensation and switched on Machine Compensation and it was very fast. This however was not ideal for me as I prefer CAM compensation so I thought I was just going to have to live with it. But from talking to Burrman and a mmoe and others on the BobCAD site on the CNCZone it was discovered that if I changed the CAM tolerance from its default 0.00254mm to 0.005mm then it would cut the time for a simple part (face, rough, finish, thread and cut off) from 2mins 10 seconds to 18 seconds.
 There is however an issue with this as well as even though I have the default and part options set to these values they will not update the current settings. This means that every time you open BobCAD you have to set the current settings again as it has gone back to the default 0.00254mm (or if in inch mode 0.0001”)  Its not a huge problem as you soon get into the habit of changing it when you start BobCAD but it is a nuisance and hopefully something that will get sorted (along with the previously mentioned  tool change dia issue) .

So that’s the niggles, as said, some have been sorted, some not . So what do I think about the way it works?
Well I must say I do like the options for choosing things such as entry moves and rapid exits moves and also the toolpaths generated are nice and seem better optimised than the current CAM I am using for my Lathe.
The workflow also seems nice and logical and once you get used to it, it is as quick as any Lathe CAM I have used.

Overall I like it and as it has much better import/export options than my other CAM I think I will be using it for my Lathe work from now on.

Next will be to start having a look at the milling side but I am sure that will also be quite a steep learning curve so it may take a while before I post my thoughts on it.

Hood

Not saving the options that you have set, sounds like there might be a file permission set to read only. Would be a nice and easy fix if that's all it is.

How did you overcome the crop circle junk gcode?
For me unchecking reversed arcs in lathe options just makes the circles appear somwhere else.

--
gallenat0r

am,
 it would seem it is a bug, I have reported it and it has been passed on to the development team.

gallenat0r
 Never really had crop circles as I had Mach in the correct mode. I tried a few of the Mach Post Processors and all produced code that would not load in Mach for various reasons but I sorted them in the post processor I made and it produces decent code now.

I reported a few things today and also requested more features. Most have been passed on to the development team so maybe they will be acted upon. One however was said to be the way it works, that was the doubling of X Tool Home dimension when in Dia mode. I was told that I would need to just enter half the value I wished so that when processed it would be correct. I knew I could do that but was hoping for a proper fix but it seems that they think it is correct. I have used quite a few lathe CAM packages and none act that way but if its what they want then so be it I suppose.
 I had thought of a way I may be able to get round it and it does work for all cycles with the exception of the grooving cycle. What I did was tell BobCAD/CAM not to do a rapid move on end of a cycle then in the PP I added a few lines to add the proper X and Z home dimensions to the respective Cycle End sections, sadly there is not one for Groove cycle so I have been unable to get that working correctly, I will keep trying though
Hood

gallenat0r

If you want to attach your xml, a bbcd file and your post processor I will have a look and see if I can get it working for you.

Hood

Well I got the groove exit rapids working via the PP, turns out it uses the End of drill cycle separate moves.
 That however now brings up an issue as it means I am calling a rapid to X before a rapid to Z for a groove but that may not be suitable for a drill cycle. The vast majority of the times it will be but I can see some occasions where it is not. I may be able to do some VB to look to see if its a drill or groove being done and apply the rapids appropriately but starting to look like I should really start dividing the X Tool Home positions by 2 in BobCAD and hope that I always remember to do that.
 If I forget I should pick it up in Machs toolpath preview and even if not then softlimits should pick it up and throw a warning but there is the odd occasion I have soft limits disabled deliberately
 Suppose I am just trying to make things idiot proof, sadly I am likely to be a higher calibre of idiot than I can proof for

 I am really starting to like BobCAD Lathe the more I use it and the more I get into the way of things, there are a few enhancements I would like and hopefully they will come out in any future updates but for now it is what it is and overall it does a good job and the tool path strategy seems to be better than the CAM I am presently using and as good as ones I have used in the past.

 Hood

I switched IJ mode from incremental to absolute in general config and that took care of the rest of them

gallenat0r

My post is set to output in Inc for arc centres and thus it is why I altered my post to add the G91.1 to the initialisation line. That is the best approach rather than just changing the default in Mach as it assures no matter what code you run and what Mach is set to as default, the code will load with the correct setting.
 I think I will actually alter my post again so that it will output either a G90.1 or G91.1 depending on what option is chosen in the PP for arc centres.
Hood

I have still not got onto testing Mill out yet, few reasons the main one being this is the busy time of year for me with the fishing boats getting slipped for their annual repair/overhaul but also as I have been struggling with a few things in Lathe.

I wanted to try and get tool holders assigned to tools and also get some tool tips (inserts) made up. I made up an insert shape for threading and that was simple to draw and assign so I then moved on to the tool holders. Drawing was no problem as I used Cubify (formally Alibre) and then opened in BobCAD. I followed the instructions in BobCADs help to try and assign them to specifi tools but no matter what I tried I could not get them working correctly, see first screenshot. I thought it may be because I was drawing in something else other than BobCAD but the problem I have is BobCADs CAD side is similar to a lot of CAD around in that it is not easy to grasp if you are used to the ease of drawing with something like SolidWorks or Alibre and I wasnt willing to spend the time to try and work things out.
 I did however see that there were a few default tool holders supplied by BobCAD so I thought I would assign one of them to see but I got exactly the same problem (see pic 2), so I then knew it had nothing to do with the drawing.

 I finally discovered the problem, the instructions given in the help file are wrong, they show the dotted circle to be at the position the insert fixes to the holder (Pic 3) and it made sense as that is how you define the actual tip (insert) however I discovered that the dotted circle should actually be positioned at the theoretical point of the insert, I moved it and it worked great but there was also a slight issue with some tools, see pic 4. In BobCAD the cutting point can be in one of 4 quadrants but for a tool such as this the actual cutting point should really be the centre, no big deal really as that can easily be offset in the drawing before the holder is assigned to a tool.

Ok so that seemd to be worked out and I now knew how to draw and assign a tool holder, I then discovered that if you use a turning tool for facing then BobCAD doesnt like that
 It seems BobCAD thinks your facing tools should have their shank running parallel with the Z axis (see pic 1) Why I have no idea as the vast majority of facing tools are actually the exact same type of tools you would use for turning operations.
 I then tried to see if I could get the tool holder set properly for facing and I rotated and mirrored the holder before assigning, worked great for the facing but as it was the same tool as a turning tool the problem was now the turning tool had the holder rotated. I could see no way around this other than to have a totally different tool being called for facing and turning operations, not really an option, so looks like I am stuck with that for the time being.
 My main reason for wanting to assign holders to tools is for internal tools and grooving tools to aid in collision detection, I have not tested the internal holders out yet but I dont see there being a problem with them but we will see.

Anyway below is a link to a video showing the simulation of a part and the problem with a turning tool doing a facing op, also shown is the insert I made for the external threading.
http://www.youtube.com/watch?v=WR9y5Wyf2fo

Hood