Need Help with BobCAD-CAM for SolidWorks V6 - Counterbore

I finally got our tiny shop to buy a HAAS VF4. Now I'm trying to make CAD-CAM efficient, and easy. Up until now, for the last few years, I've been making the models and prints, and then punching them in conversational on a ProtoTRAK machine...

As much as I'd love to use Mastercam or Gibbs (Ideally, something that will plug into SolidWorks), the money's not there. We purchased the latest version of BobCAD-CAM for Solidworks, version 6, but I've been struggling.

I'm relatively new to CAD-CAM, although I've been working on SolidWorks for the last 2+ years, and I can make models decently. I understand the basic idea, but BobCAD is ridiculously clunky, and we're not going to spend 3x the software cost for a 2-day course that covers a lot of stuff I'll not be using.

Currently, I've been programming longhand. It will get the job done, but it's tedious to do small jobs, and it's going to catch up when I need to do more detailed projects. So, I've been working on BobCAD for simple projects.

The current project has 8 tapped holes, 4 counterbored holes, and a large hole in the middle. I was able to get BobCAD to pick up the 8 tapped holes, and have it working in Simulation. However, every time I try to pick up the 4 counterbored holes, it won't recognize them in the "select geometry" feature. I've selected, separately, each feature of the counterbored holes, from the top, the sides, edges, the bottom, everything. Nothing works.



I attached a photo of the part. You can see the toolpaths for the tapped holes.

Any ideas? It'd be decent software if it'd work a little better. If I don't tell each individual feature to compute the toolpaths, Simulation won't work. One would think selecting "Simulation", it'd automatically compute toolpaths via the selections entered.

Any help would be great.

If you still have support, give them a call. There is likely a very easy way to do what you want to do - you just don't know it yet.
I can't tell from here if all your geometry is good. If there is an error in the geometry, stuff doesn't work. (not that I'd know anything about that, haha)
I use just enough CAD to get the system to create the CNC program. Looks like you are going at it from the opposite direction. (I don't use SW at all) To me, punching programs into a control is VERY inefficient if I already have a drawing on the confuser.....

Get some training - the BobCad training is actually reasonable priced IMO.
Good luck!

I use Bob,but not V6 for Solidworks

That said,in using just Bob you can CAM either by selecting geometry from 2D or 3D solids.Which way is failing you ?

Have you tried both ways ?

Bad geometry is highly suspect,but need more info to know

If picking using 2D,all that is necessary to CAM your program is "points" where the center of each c-bore is.

The advantage of a solid model is you do not need to fill in all the data of diameter and depth

So might try the fail safe way and just select points and enter the data for parameters

Thinking geometry issues with your drawing is what is failing

Download HSMXpress, it is free and you can easily program your part. It is only 2.5D. You can download numerous posts for free. You also get free tech support from the Autodesk cam forum.

You probably already figured this out as it's been about 3 weeks since you posted this. But if you haven't or for anyone elses general information. In V6 to use the Mill Counterbore Hole feature, to select the counterbore geometry, you check the box for Select whole bodies and BobCad will automatically select all counterbored holes in the part. Then you can modify any of the dimensions you need to to make the holes as you need them. Hope this helps.

This was days ago but I just joined this site and looking for some help and this was the forum page that I found the site on so I thought I would put my opinion in here for anyone else who comes looking. V6 needs to use solidworks sketches quite heavily to really work right, clicking model surfaces is just asking for trouble for anything complex until you get to 3 axis milling. While I usually mill my counter bores, drill cycles of this sort are best done by creating a sketch over your model face and putting points on each of the center points of your drill holes.

Each different set of holes should have a different sketch, so all your 1/4" holes should be one set, all your 3/8" holes and so on that way when you go to create your CAM pathing you just select the correct sketch and you get all the right holes.

Also due to an issue that I have yet to see resolved (I talked to support yesterday about it and they said it still wasn't solved in V8), any time you update your model, Bobcam will ask if you would like to readjust your geometry or something of that sort, if you hit yes, all of your depth data will be changed to whatever bobcam thought the default was, which is usually the height of your sketch plane, so it can be very beneficial in the long term to create your sketch planes at your max depth of cut.

-Andrew