[ksanalytical]

I've been searching around and don't see anyone else talking about this so I'm assuming it's my own ignorance here, but i have the worst time getting a profile chamfered with BobCAD v24. I suspect that I'm misunderstanding something in the parameters which is causing dramatically erroneous result. I find myself simulating over and over again until I finally tweak it in. I don't use it much, but on a given part, I probably spend 3 times as long setting up a simple chamfer as every other toolpath combined.

I've attached a pic of the page. I'm using a 0.375" 120 deg mill/drill. The only thing I can find blatantly wrong seems to be the chamfer angle field value vs the diagram. You'd expect to enter 60 degrees based on the diagram but that's definitely wrong. It seems like the program has all the necessary data to do the same trig that I do externally and I can't imagine that they wouldn't have built it to help users avoid the extra hassle.

Base on these parameters and a profile running along the Y axis at X=0 to go to X=-0.0875" and Z=-0.0895" and move straight along the Y axis. Instead, the cutter goes to X=-0.032 Z=-0.177. Am I crazy? Is my trig that bad? Even so, what on earth is the "cutter position" doing anywhere other than X=-0.0875? Incidentally, if I set the "cutter position" to zero, I get a tool path right along the line. If I set it to 0.01, I get a toolpath offset by 0.0169.

I apologize if this has already been gone through. I'm even open to the idea of upgrading to V25 if it sorts any of this out, but it feels like this is something simple.

Best regards,

Ken

[Jessebobcad]

If you hit F1 on your keyboard while in a feature it brings up the help system for that page.

I have pasted the definition for Cutter position:
Cutter Position - This field specifies a distance away from the center of the toolpath to begin the cut, in order to use a chamfer tool that does not have flutes that extend all the way to the tip.

The picture is wrong when you click in Cutter Position.

It is the amount of shift you want the tool to move if you don't want it to be right on the edge of the flute. Remember this distance will be added to depth. When you shift over this will also shift down. This is used to change contact point for cutting.

On a pointed tool the image is correct.

[ksanalytical]

Jesse,

Thanks for the clarification on the "cutter position" field. That would have tripped me up eventually. I'm almost always using pointed tools though so that shouldn't be the source of my error. A few things from this morning:

1) For whatever reason, Help does not appear when I press F1 in the feature edit screens. The regular Help function works fine though and I have read through that enough that anything I'm missing is never going to become apparent.
2) I understand and would expect the tool to move further down in Z when the cutter position field is increased. I noticed this morning though that this seems to be applied as a fixed offset rather than calculated. A 0.1" cutter position offset pushed the cutter out 0.1" and down 0.1". That's correct for a 90 degree chamfering tool, but completely wrong for any other tool. Again, the math on this is so simple I can't believe anyone would have coded that function for a fixed offset, but it seems to be acting that way for me. The tool selection shows 120 deg and the parameters dialogue also shows 120 degree (not sure why is needs to be re-entered, but at least you know they match). I've played with 0, 0.1 and 0.2 "cutter positions" this morning and they move the tool down by the same fixed offset no matter what the angle is.

More testing just now. I drew some lines off the profiles to show various chamfer angles. This allowed me to change variables rapidly and verify if the cut would work right or not simply be seeing if the toolpath lined up with one of those angles (sharp tools only). I found that the magic bullet was not anything in the "parameters" section, but rather the tool diameter. At 0.5" diameter, I should have had enough tool to cut a 120 deg chamfer at the total depth of my 0.114" stock even with a 0.05" "cutter position" value. Moving from sharper to broader chamfer mills moves the toolpath away from the stock as it should. However, as soon as I pass ~100 degrees of chamfer angle, the tool path starts moving back toward the stock again. I found that I could eliminate this effect by telling BCAD that the tool diameter was much large than it really is. Do you have any idea how Bcad uses tool diameter to restrain the toolpath on a cut like this?

It seems like BobCAD is requiring some minimum clearance from the total diameter of the tool which limits its effective diameter. This number appears to be 0.1" from the max tool diameter to the start of the cut (I only checked a 0.57". This could be a % of diameter, but I doubt it due to the odd numbers I was using to determine it.). That effectively reduces the useable diameter of the tool by 0.2". I could understand that (even though it's completely unnecessary for mill/drill cutters), but the fact that the calculations go all crazy when this is surpassed confuses the heck out of me. I'd like to use these mill/drills to cut large chamfers in multiple passes but that's going to get alot more complicated if I can't put the tool right where I want it without resorting to jacking with the diameter. Based on my earlier tests, it almost looks like BCAD forces a 90 degree cutter angle once you pass the diameter limit (guess). That would explain why the erroneous toolpaths dropped by the "cutter position" value in Z and X equally.

In any case, thanks for the suggestion and I hope this will be helpful to someone else down the road. The solution for now will be to tell BCAD that my 0.375" cutter is actually a 0.5" and wait till that comes back to haunt me. That is unless you've got a better suggestion.

Ken

[Jessebobcad]

I would recommend calling in to support at 727-489-0003 or send them an e-mail with the above to [email protected] so that they'll be able to assist you with this a little faster.

[The Engine Guy]

I've been searching around and don't see anyone else talking about this so I'm assuming it's my own ignorance here, but i have the worst time getting a profile chamfered with BobCAD v24. I suspect that I'm misunderstanding something in the parameters which is causing dramatically erroneous result. I find myself simulating over and over again until I finally tweak it in. I don't use it much, but on a given part, I probably spend 3 times as long setting up a simple chamfer as every other toolpath combined.

I've attached a pic of the page. I'm using a 0.375" 120 deg mill/drill. The only thing I can find blatantly wrong seems to be the chamfer angle field value vs the diagram. You'd expect to enter 60 degrees based on the diagram but that's definitely wrong. It seems like the program has all the necessary data to do the same trig that I do externally and I can't imagine that they wouldn't have built it to help users avoid the extra hassle.

Base on these parameters and a profile running along the Y axis at X=0 to go to X=-0.0875" and Z=-0.0895" and move straight along the Y axis. Instead, the cutter goes to X=-0.032 Z=-0.177. Am I crazy? Is my trig that bad? Even so, what on earth is the "cutter position" doing anywhere other than X=-0.0875? Incidentally, if I set the "cutter position" to zero, I get a tool path right along the line. If I set it to 0.01, I get a toolpath offset by 0.0169.

I apologize if this has already been gone through. I'm even open to the idea of upgrading to V25 if it sorts any of this out, but it feels like this is something simple.

Best regards,

Ken

Ken

I think you are being thrown a little by some of the terminology used, it isn`t actually that complicated and if it`s any consolation quite a few CadCAM softwares do struggle a little with the Chamfers

1) The angle is always the "included" angle that is shown at the Tool info dialog so 120 deg is 120 deg in the feature, some softwares do use the "half tool angle" but not BobCAD.

2) the "Tool Position" is just there to allow the user to adjust the point where the material touches the flutes, so for example BobCAD may default the cutter to cut with the bottom edge of the flute exactly on the edge of the material, now if there is a very small rad or the tool is a little worn you could end up with a small step on your chamfer, not desired at all, by using the "Tool Position" box you can move the centre of the tool out a fraction to avoid this, now normally just moving it out would change the chamfer width/depth etc but BobCAD also moves the tool down a fraction so the end chamfer is still correct, pretty neat I always set the "Tool Position" to 0.000 run the Predator Backplot sim from the G code and then if I think I need to make any adjustment it`s a quick and easy mod. If you are anything like me you won`t have dozens of chamfer tools so it soon becomes easy to remember just how much to adjust for each tool

Attached are a couple of images of sharp tool and flat bottom tool and the BobCAD program that produced them
Hope they are of some help to you

Attachment 192336Attachment 192334
Attachment 192332

Regards
Rob

[RAF.]

Rob
when you enter a 60 deg. or 120 deg. pointed tool do you have to give the small dia. at least .001 so it will accept it? That is what I am having to do.

[The Engine Guy]

Rob
when you enter a 60 deg. or 120 deg. pointed tool do you have to give the small dia. at least .001 so it will accept it? That is what I am having to do.

Hello RAF

No, I don`t have any problems like that, I am on V24 Build 546

Regards
Rob

[RAF.]

Hello Rob
I just tried it in my V24 build 546 and yes you are right it accepts it not problem but with my V25 build 996 it asks for an amount larger than 0 for small dia. when creating a new tool.

Thanks Much
Roger

[The Engine Guy]

Hello Rob
I just tried it in my V24 build 546 and yes you are right it accepts it not problem but with my V25 build 996 it asks for an amount larger than 0 for small dia. when creating a new tool.

Thanks Much
Roger

Roger

Just tried it in my V25 Build 895 and I can input 0.000 without any problem, don`t know about Build 996 as I had some issues with it so I rolled back to 895, not had any problems since

Regards
Rob

[The Engine Guy]

Hello Rob
I just tried it in my V24 build 546 and yes you are right it accepts it not problem but with my V25 build 996 it asks for an amount larger than 0 for small dia. when creating a new tool.

Thanks Much
Roger

Roger

Just as an afterthought, have you tried resetting the small diameter to the 0.000 value on the Parameters Dialog page down in the lower right, I can get V25 to alter the tool info by changing the value there, if it is "greyed out" just toggle it between flat and sharp tools to get it editable. Also it only appears to do it with Chamfer Mills and not with Chamfer Tools

Regards
Rob

[ksanalytical]

Rob,

Thanks for the input and advice. When I bought BCad, I was told by another user that Predator was essential and should not be skipped. I think it's saved me my weight in Al at this point as many times as I thought I had things right only to find that something was WAY off when it actually came time to cut. I haven't called in for support yet, but I do plan to talk to them because my difficulty was not with these "normal" chamfers wherein the user is just knocking the edge off. I need to create a much larger chamfer that is completely within the geometric capabilities of the tool, but the toolpath can't be calculated. Just as you mention the "cutter position" creates an offset from the tip (or the small diameter for flat bottom tools), there seems to be a limitation on the top (widest part of the tool) which is fixed. My testing showed that one can only cut a chamfer with width equal to the tool radius-0.1"-"cutter position". I've gotten good simulations on my parts by telling BobCAD that my chamfer mill is much larger in diameter than it is, then changing the tool value in Predator to the actual tool diameter. The cut is fine, it just violates some internal limit in the software. I don't think they're going to write a patch at this point so there's not much point in worrying about it now that I have a work-around.

Thanks again,

Ken

[RAF.]

Rob

Yes! by changing the value in the Parameters Dialog page it did work

Thanks Much
Roger

[LeWhite]

Flat bottom chamf

[LeWhite]

Yup the picture is wrong. The picture does make sense so the math must be wrong. Seems to add tool offset to half tool dia. Thats especially wrong for combo front /back chamf tools. Seems to work if you know the flat botton radius of the picture and enter 0.0000 for the tip dia. Dont trust it one bit. Bob said it was fixed with last update of 996, but its still here