[cnczoner]

I need to make this thing that looks like a cup with one side cut off and with the stud in the middle.



Creating the 3D model is simple, but to get g-code I pretty much re-created a 2D version of it so I could use the pocketing feature. And I created contours for the edges of the pocket area, and also the stud in the center.

When trying to create the toolpath, Bobcad (v22, btw) would crash at first, but I enclosed the inside pocket area with some lines and arcs, and now I can create the toolpath and g-code. But the g-code it creates wipes out the stud in the center. I am selecting the stud as part of the geometry. I can't figure out how to tell it to not mill that area out.



Also, the code won't verify with Bobcad's verification tool, so I am using an external tool called cncsimulator to verify.

Anyone know how to get around this?

Thanks,
-Neil

[LeeWay]

I don't use Bob Cad, but that should be really easy in 2D. A C and a dot. A single pocket should take care of the inside and leave the island. I have to make sure the center dot or island is on the same layer as the C. I use Turbocad and Sheetcam.

[cnczoner]

Before purchasing Bobcad, I did experiment with Sheetcam and was impressed with how easy it is to do things in 2.5D (which is what I really need), but I felt I would go with a 3D program so that I could visualize the part easier (as above, which I could do previously using emachineshop's software). But it was first a major letdown when I found out that after creating a 3D model, I had to pretty much extract a 2D projection of it and then specify depths as I would with a 2.5D program such as sheetcam.

In the meanwhile, I found out that the shop that does my machining also has a copy of Bobcad and to get this part made sooner, I figured I'd give them these models, but they too could not generate g-code from it. They use SolidWorks otherwise, but they don't have the time right now to re-create it in Solidworks.

I could've written it manually already, but I need to learn to use Bobcad, so hopefully someone familiar with Bobcad will set me straight here.

Cheers,
-Neil.

[tjones]

It seems to work well.

First off I did not select a start point. However if you do then select one outside the geometry where the opening is.

Also select the path to go from outside to inside to get the cut to start ouside of the part. Also the path will start based on the middle of the first segment in yoyur contour. You can also break (devide) a segment to allow controll over the start position.

This test also has a finished frofile pass after the pocket.

If you wish to do this from a solid model then you may wish to get the version with Z level roughing.

[jimalb]

I just did this with my BobCad v22 and it works just fine for me. I drew this as a 3d model and did an Utilities>Extract Edges>From Solid, then blanked out the solid so I could see the edges then went through and deleted all edges I did not need then did cam tree and did Mill 2 Axis>Pocketing and selected the outside shape and selected the inside shape and then generate the code. It preserved the inside post and cut out the pocket just fine and verified OK too. If I knew how to post the screen pic like you did I would Put It this post to show better how it looks on my system. But My guess is your not getting your inside post selected as part of your geometry so BC is cutting the post out of the part.

[cnczoner]

Thanks for the replies.

I've been experimenting and experimenting, and I've come up with a revelation -- I am selecting the center post properly, but it retains the center post only if that post has a radius of 0.0875" or larger. Anything smaller gets wiped out. I'm still experimenting to see if any other parameter changes this value, else it would have to be a bug. I can't see why there would be a magic value such as this.

[cnczoner]

Okay another revelation -- it seems that with an inner wall dia of 1.675", center stud diameter or 0.1", and cutter width (overlap) set in the pocket operation to 50%, it wipes out the stud. If I change to 30% it keeps the stud. 60% or 65% keeps it, 75% wipes it out. Huh!?!?!?!?!?!?!?

[jimalb]

OK, I just redrew With a center post of .0625" radius and it worked fine for me, then redrew with a .006 Radius and still shows to be cutting, I did find if I selected a start point it would wipe out the post for some reason, also when I made some changes I had to delete the feature pocket and then recreate it or the tool path would wipe out the post still, Mabe some bug but by deleting and recreating it, it would redraw the path correctly. ???

[cnczoner]

Thanks for the help guys. More revelations, but I'm not sure if to call it progress...

First, with the right (by trial-and-error) combination of stud diameter and overlap, I get this...



The problem with this is the little "triangle" path under the stud, which translates to an incorrect path. (I am using only a roughing pass by specifying a zero side allowance in the pocket parameters). CNC Simulator gets me this (which shows that the path is wrong)...



I noticed that you (tjones) also have the triangle path, but you're using a finishing pass, so I set a side allowance of 0.05 to get a finishing pass, and I get this toolpath, which now seems correct...



CNC simulator gets me this ... finally! ...




But the "random" setting of cutter width to get it to leave the stud is disturbing, and obviously a bug, unless someone has a better explanation. Then I don't want to use a finishing pass, but not sure how to work around this. And predator still won't verify this in Bobcad, so I have to use CNC simulator to verify. Yes CNC simulator is free, but it does not recognize subprograms, so I have to move things around each time I verify, and I made sure I got Predator when purchasing Bobcad for a reason. And btw, I'm still using Turbocad to draw things and extract coordinates since Bobcad's 2D drawing tools are considerable basic.

Seriously, with Turbocad and Notepad, I could've written the g-code already. Anyone from Bobcad care to comment...??? I don't think calling support will do me any good since I called once a few weeks ago and was told that "crashing *is* expected behaviour ... if I do something incorrect". No, that's what error messages are for. How are people using this in a production environment. No wonder Bobcad's sales folks kept saying they got sued for people trying g-code.

Frustrated,
-Neil.

[cnczoner]

jimalb, I'll try that tomorrow. Spent tooooo much time on this already tonight.
Cheers,
-Neil.

[cmmachine]

I have recently acquired V22 and haven't had much time to experiment. I know with earlier versions you needed to select your outside edge of pocket in one direction and the island or in your case stud in the other direction to leave the stud/island. I've used bobcad since V17 and have had great success. I do have the training cd's for V22 so maybe tommorow I'll take a look @ generating g-codes from a 3-D model.

Mike.

[tjones]

I also was able to get the wipe out with 50% stepover. (I have some basic settings that I use and most likely this is why I did not see this the first time) It does seems that the % of cut has an effect on the output and I would also call it a bug. I think I will report it to tech.

Also I would not say that any software crashing should be considered normal. Crashing is caused by the software doing something that can't be done in the way it was programmed. This is why a programmer adds error checks and yes "User error messages" to tell you not to do that. Or limits added in the code to prevent it.

Since Bobcad is still working on adding features and operations I give them a little understanding. But I would think telling someone that it is normal would be the wrong thing to say. Maybe the person you talked with is getting numb to the whole testing procedure (nuts).

As for not being able to simulate I am not sure why. My Predator works good. I am not using subs though and maybe that has an effect. try turning off the subs to see if it simulates then. If not then I would guess soemthing wrong with Predator or it needs updated to the latest release.

BTW: My little triangle works just fine. Do you have any cutter comp? When roughing I do not use comp but let the path take care of it. This may be a post issue and not a software one. Maybe but maybe not.

[tjones]

I guess what I have done that avoids many of these issues is to save templates of my normal features and settings. By this I mean I have determined what has worked and saved them to a name like "pocket with finish pass".

Then I can open that file and all the seetings are saved. I simply merge my part or draw a new ne and select the geometry. Makes for a very fast post in the working environement.

[bjcnc]

I too could not verify check out FAQ 12 Settings stock geometry pdf on their website. It does work when you do it that way. Basically all you are doing is drawing a rectangle around the drawing so that a stock piece size can be seen by the simulator. You will need to set thicknes under mill stock. I too wish someone would give a step by step a lot of time has been wasted trying to figure out what and how . I too am having problems cutting off design parts I will be following this thread closely hope you can understnd what I said and that it helps you.Good Luck bjcnc

[cnczoner]

I've used the verify feature before, so I went back to some old test files I had and could not verify those now. So I re-installed Bobcad and I could verify successfully. After some more use, Bobcad crashed a few times and I later realized I could not verify again. Reinstall, and verify works again. So the crashing is causing some file corruption. Arrrggghhh!!!!

[cnczoner]

...
Also I would not say that any software crashing should be considered normal. Crashing is caused by the software doing something that can't be done in the way it was programmed. This is why a programmer adds error checks and yes "User error messages" to tell you not to do that. Or limits added in the code to prevent it.

Oh believe that I know this well. I've been a software developer for years and I've worked for MS, IBM and other major players. I know what proper software is.

And a few days later, I get a letter in the mail requesting money for a software support contract. (nuts)

Since Bobcad is still working on adding features and operations I give them a little understanding.

But if that's the case, then not telling me this up front when begging me to buy their software is misrepresentation. Most beta-software I've used (and properly identified as such) has had less bugs. I got long spiels from "Kenny" about how long the software has been around and how great and advanced it is now.

BTW: My little triangle works just fine. Do you have any cutter comp? When roughing I do not use comp but let the path take care of it. This may be a post issue and not a software one. Maybe but maybe not.

I have not set any cutter comp and not aware of how to do this other than telling it the endmill size in each operation. That's the only compensation I've used. Are you suggesting there's another place to set compensation?

Cheers,
-Neil.

[cnczoner]

BTW, for the part for which I was trying to create the g-code, I ended up drawing it in Turbocad and wrote the g-code manually by extracting dimensions from that.

[tjones]

Yes,

Cutter comp is actually a code output. So if Bobcad generates a paths that comps for the endmill and also there is cutter comp turned on then the simulation will be a little weird.

Some people do this intentionally to comp a few thou at the machine when their endmill does not match what was programmed in the CAM package.

I do not know if this is the case for your problem though.