[Ben S]

Engine Guy, thank you for the detailed response. I will have to take some time to go over the post and see if it includes the lines you highlighted. I'm not experienced at reading posts so that will take time. It is a default post that came with the software, though, so I would think it would be set up to work with the features in the software, right?

As to my finish pass question, I use tools that have the same cutting diameter and shank diameter. If my feature is deeper than the flute length I cut several roughing depths. If it cuts only one finish pass at full depth then the shank will interfere with the wall above. But if it cuts a finish pass at each depth then there is no problem. Make sense? In Mastercam there is a check box for this. I'm not seeing a way to do it in Bobcad.

Thanks for the input.

[mmoe]

Engine Guy, thank you for the detailed response. I will have to take some time to go over the post and see if it includes the lines you highlighted. I'm not experienced at reading posts so that will take time. It is a default post that came with the software, though, so I would think it would be set up to work with the features in the software, right?

As to my finish pass question, I use tools that have the same cutting diameter and shank diameter. If my feature is deeper than the flute length I cut several roughing depths. If it cuts only one finish pass at full depth then the shank will interfere with the wall above. But if it cuts a finish pass at each depth then there is no problem. Make sense? In Mastercam there is a check box for this. I'm not seeing a way to do it in Bobcad.

Thanks for the input.

There isn't the option to do this automatically within a pocketing feature or profile feature. You can do it in two steps though, and you have to sort of trick Bobcad into doing so. I also use V24, so this should be pretty much exactly the same for you.

For a pocketing feature:
First, go to your cam tree and right click on "Milling Tools", then select "Part-->Tool Pattern". This will bring up the lists where you can select how each feature will operate. You then click on Pocket which will display the operation lists. To the left you will see "With Chamfer" and to the right you will see "No Chamfer". You can highlight any operation and delete it with the "Delete" button below that list. Personally, I rarely need to chamfer anything, so I've set up the "With Chamfer" side to have only the "Endmill Rough" operation while I've left the "No Chamfer" side alone in case I want the option of a full height finish pass. You could also set up the "No Chamfer" side to only have "Endmill Rough" if that's more convenient for you. From now on, you can produce a roughing only pocket routine. If you want the change permanent, you'd have to go the "Milling Tools-->Default-->Tool Patterns", but I'd suggests saving the default tool patterns to a backup file first in case you wish to restore the factory settings.

Next, start a CAM window for 2d pocketing, select the geometry and then either check or don't check the "Chamfer" box depending on how you set up the above so that you have a roughing only feature. Now, you can set up the operation as normal for the tool, then in the "Patterns" window check "No Profile" along with any other preferences here. In the next window, "Parameters", set the side allowance to whatever you want to remove with your finishing pass and the bottom allowance to "0". Check "Multiple Steps" and set them to your preferences, then do the rest of the windows as normal until you click "Finish". This will produce a pocket without a finish pass, but also with an allowance on the sidewall which can be cleaned up with a profile pass. Actually, to be more correct, it will still produce a finish pass that will cut air, but it will be located within the pocket you already roughed out, so there will still be material to cut for a finish pass (not sure why it still insists on generating that profile pass, but it does). Now you would start up a CAM feature with 2d Profile, and make sure you do the roughing pass with NO ALLOWANCE. This will allow you to do multiple steps down as if it's a finish pass and the profile feature will automatically skip the finish pass that it would normally do if you set an allowance.

If it's a profile pass, you can go into "Milling Tools-->Part-->Tool Pattern" again and set the "Contour" feature to have only a "Endmill Rough" pass. At this point, you now have to do two different features. One with an allowance, then the next with no allowance. You can set them both to have multiple passes as needed.

All that said, and without seeing the parts you're working with, it may also be a good idea to add another piece of software too your computing toolbox. I've started using EstlCAM 2.5d, which costs $25 (no joke), to produce some of these toolpaths that don't fit into the standard Bobcad workflow. Bobcad offers more overall and it's price reflects this, but when it comes to 2.5d work off of simple 2d DXF drawings, EstlCAM is a great addition to fill in the gaps. In the tool setup for EstlCAM, you can define the maximum cutting depth per pass for each tool, which means that as you generate tool paths it will automatically take the max depth into account and you don't have to do anything special. You also define things like the amount of overlap, which it will then apply as specified for each tool automatically as well. The post processor system is very robust and easy to work with to customize. The tools are easy to use and there are a lot of tools Bobcad simply doesn't have such as automated tabs and the ability to select the start point. Other things are missing or don't work quite as flexible as Bobcad (such as won't do a rough then finish pass for profiles, but does clear out pockets and follow with a finish pass), but for most 2d work I find that EstlCAM is a bit more efficient to use. There is a demo available, but really for $25 it's hard to go wrong with it and I think it's cool to support individuals who create good products with new ways of looking at these things. Coming from Bobcad, you can learn EstlCAM in a day no problem, if not a couple hours.

[Ben S]

Thanks for outlining the work-around mmoe and I am downloading the EstlCam demo now. I appreciate the help.

[mmoe]

Thanks for outlining the work-around mmoe and I am downloading the EstlCam demo now. I appreciate the help.

No problem. Keep in mind that EstlCAM is very different in how it looks, but that shouldn't be confused for it not being any good. I may see if I can put together a quick video of how it works, but I'd also recommend watching the video the developer made as well. Just keep an open mind, it's not like other CAM systems in appearance but it's quite capable. Part of what makes it look odd (compared to most CAM systems) ends up making it easy and fast to use.

[Louis Roy]

Hello all, I am probably to late with a reply but I will anyway. One thing I noticed was the finish tool lead in was vertical, from my experience a vertical lead in is not the right way to go if you need cutter comp, it allows for no movement to activate cc. Also under finish patterns, comp setting are system comp on, machine comp off, using these settings BobCad is going to offset the toolpath for half the tool, but not give you any adjustment for the machine. System comp off, machine comp on, will give you G41/ G42 but not with a vertical lead in try one of the others parallel, right angle or circular.

I used V25 and the generic HassVF mill post. I don't have V24, so this may not be a valid answer for this question. I hope this helps.

BobCads cutter comp system was very hard for me to figure out, the V25 Mill Training video series disk 2 video # 88 at about 5 minutes in explains it pretty clearly