Turn off center drills?

[cnczoner]

How do I tell Bobcad v22 to only drill in one pass and not center drill? There are feature operations called "drill --> center drill" and "drill --> hole", but they both include a center drill operation.

Thanks,
-Neil.

[tikka308]

I have not found a way to do so (although there certainly may be a way) - and thus I usually just manually delete the GCODE. It's definitely not the most convenient solution, but it works...

[moldmker]

In the CAM feature tree:

CAM Part>Rt. click Milling Tools>Part>Tool Pattern:

Click on Hole in the menu and you can delete Center Drill from the pattern.

If you always want it that way, pick Default setting rather than Part. Be sure to save when you exit Bobcad.

Good luck.

[cnczoner]

That works. Thanks!

[Malish]

I saw this post yeasterday and thought I would try it. It works great. My question is though, can the same thing, or something simular be done with the milling process profiling, so that I only get a roughing pass and no finish pass? We do some parts out of thin plastic sheets that a finish pass is not needed.

I tried to modify the the milling profile setting but it says "can not edit". Also there is a "milling" setting listed in there that has just the rough pass, but I don't have that to pick from when I add an operation.

Anyone have any ideas on this?

[tikka308]

In the CAM profile of your cut (i.e. pocket), in "parameters", if you remove the side allowance (mine defaults to 0.05"), it will remove the finish pass

[Malish]

ummmm...DUH! I will go slap myself upside the head now.

Thanks!

[seanreit]

Can you change the default to zero?

[Allen123]

Another thing you can do is leave a finish amount and just zero the finish tool. By doing this the software will not call a finish cutter and leave stock so you can run a profile feature for the finish.

You would want to do this so you can use cutter comp on the finish pass. Right now in a pocket BobCAD will not post cutter comp on the finish pass it offsets for center line. I think this is something they are working on, but who knows when it will come to light.

[Shawn Lucas]

How do I control the depth of the center drill?

[moldmker]

How do I control the depth of the center drill?

That's a good question.

Apparently the software calculates the depth and is unchangable in all but the Center Drill Feature.

However the default tool parameter for center drills has zero pilot length and point angle (unless I changed mine and don't remember).
If you go to Cam Part>Milling Tools>Tools>Center Drill you can define center drill geometry that will change how the depth is calculated. This can be done in the Feature itself with Manual Tool definition but be sure to verify your G-code if you use Manual Tools.

If you alter the machining order as discussed earlier in this thread and call the Center Drill Feature manually, then you can over-ride the depth.

moldmker

[laserkey]

Go to cutting conditions and you can tell how far you want it to chamfer each time. far as the not using a finish pass . You can do the edit on the feature and then right click on it and click on "save feature" and then the next time you want to call that tool you can right click on the milling stock and tell it to load that end mill feature and now you only would modify the depth you want . it will pick out the correct feature and all .
Very neat stuff.
Need help call 281 932 6526
If you have not bought the videos or recieved them for free it is a must.