BobCAD 3D mill in hole not reaching full depth

[RamseyRuss]

Using BobCAD V32 I am trying to 3D mill a taper between two hole diameters. I am using a Z-level finish operation. It is tight - I am trying to use a 3/16" ball end mill to taper from a 0.266 hole to a 0.257 hole. The tool path does not make it deep enough to complete the operation. If I use a 1/8" tool it will work. (Note, the toolpath is possible with the 3/16" end mill - Surfcam does it fine, but I have BobCad.) Is there some sort of tolerance setting that I'm missing? I can't find anything that seems to make a difference. I have also tried a bull nose tool and a flat end tool - they look even worse (but all are probably milling just as deep, considering the point of full tool diameter).

Similar Threads:

• Need Help!- AASD servo not reaching full rpm in speed mode.
• Full Depth of Tool
• CNC XY Mill Drill Lathe Table. Mach3 BobCad Full 4 Axis
• CNC XY Mill Drill Lathe Table. Mach3 BobCad Full 4 Axis
• CNC XY Mill Drill Lathe Table. Mach3 BobCad Full 4 Axis

[BurrMan]

Using BobCAD V32 I am trying to 3D mill a taper between two hole diameters. I am using a Z-level finish operation. It is tight - I am trying to use a 3/16" ball end mill to taper from a 0.266 hole to a 0.257 hole. The tool path does not make it deep enough to complete the operation. If I use a 1/8" tool it will work. (Note, the toolpath is possible with the 3/16" end mill - Surfcam does it fine, but I have BobCad.) Is there some sort of tolerance setting that I'm missing? I can't find anything that seems to make a difference. I have also tried a bull nose tool and a flat end tool - they look even worse (but all are probably milling just as deep, considering the point of full tool diameter).

Zip and attach your bbcd file and i'll take a look.

[RamseyRuss]

Zipped file is attached (I think), thanks for taking a look.

[BurrMan]

How deep did you want that to go? How deep is "complete the operation"?

[BurrMan]

Hey RamseyRuss,
So I kindof went over it a bit just to get a feel. Your transition taper happens pretty quick there, But I don't think that is limiting you.

For some reason the tolerance of .0005 is interfering with that transition. It has the toolpath stop about half way through that 1 transition part.

Setting the tolerance of the machining operation to .0001 will allow you to go all the way!! (Thats in the ZLevel Finish Feature on the Parameters page)

Also would shrinking the tool diameter, but this is not a desired option.

I didnt really start crunching numbers and checking tool geometry fitting with the surface geometry parameters for an answer as to WHY the larger tolerance of .0005 wont go past that point in the calc. I just dont have it in me anymore.

If you wanted an in depth look for understanding so you can move forward with a better insight, I could suggest the BobCad forum as you can get responses from even BobCad Devs there.

Anyway, Onward. Good luck!

[BurrMan]

Added Note:
Something about that particular geometry selection and boundry selection causes the toolpath to start stepping off about halfway down. (If you look at the toolpath from the top view it is easier to see that)

Most of that selection is sortof not needed for that toolpath anyway. So I fixed that by removing the boundry and geometry selections, then selecting "Just the 3 inner surfaces" for the geometry of the ZLevel Finish and it didn't step and completed nicely (Defined tool gave collision errors in the simulation when hitting full depth, so you have to look at that...)

Personally, I would head over and get some input from the other forum. ( just because i like to have the answers )

Maybe Al will see this here and help out..

Anyway.....

[BurrMan]

Second added Bonus!!!
Just for fun, I'll attach a new surface here.

Your original hole just had a G0 loft in that second surface down, the actual transition from .266 to .257

So here is a file where i made a G2 Blend between that first surface and the third one, to give you a smoother transition....

Just use "Merge" to bring it into your file and replace the old Cylinder.

Not needed obviously, and may even be wrong for your application. But I had already made it in some tests, so just giving it up here...

[RamseyRuss]

Wow, that's a lot of information, thanks!

My first operation (drill and ream) puts in a .257 hole, so the depth I'm trying to mill is just far enough to create the .266 hole to a depth of .250, and then the taper (1.5 degrees) to .257 - a bit over 0.4 total.

I will change the machining tolerance as you suggested and see if I get the desired result.

I had started with just the three surfaces, but was getting toolpath on the outside of the surface (inside the cylinder). Someone on the BobCAD forum suggested just selecting the solid model - but that wasn't the whole issue.

I don't understand the G0 loft and G2 blend terminology, but I will take a look at what you sent and see if I can see the difference.

I had started out on the BobCAD forum, but wasn't making any progress; one guy, that appeared to be a BobCAD dev. just told me that I would have to use a 0.125" tool.

Again, thanks.

[RamseyRuss]

I tried the merge you suggested, and just looking at the file you sent - I'm afraid I don't see what the difference is.

It bothers me that, even with the 0.0001 tolerance that you mentioned, when I post the toolpath I get three G3 moves (X,Y,I, and J) at every Z depth rather than one simple G3 circle (I and J) at each depth. Plus, if I pick just the upper two inside surfaces (the only part I'm really trying to mill) and a ball nose end mill, the toolpath stops with the ball tip at the bottom edge of the second surface, rather than extending below it as is required to mill the full surface (doesn't matter whether I use Tool Tip or Tool Center in the parameters). Guess I will try again on the BobCAD forum, as you suggested, and see if anybody else picks this up.

[BurrMan]

I tried the merge you suggested, and just looking at the file you sent - I'm afraid I don't see what the difference is.

It bothers me that, even with the 0.0001 tolerance that you mentioned, when I post the toolpath I get three G3 moves (X,Y,I, and J) at every Z depth rather than one simple G3 circle (I and J) at each depth. Plus, if I pick just the upper two inside surfaces (the only part I'm really trying to mill) and a ball nose end mill, the toolpath stops with the ball tip at the bottom edge of the second surface, rather than extending below it as is required to mill the full surface (doesn't matter whether I use Tool Tip or Tool Center in the parameters). Guess I will try again on the BobCAD forum, as you suggested, and see if anybody else picks this up.

I just posted a quick video over there for them to see. It will also a better ploace to get the answers about the posted G3 and how those can be controlled or what not. I dont really know Gcode very well.

The video has a tidbit at the end to show you continuity in an exaggerated way.. You should probably just ignore that part of my response. It doesnt seem very relevant to what you need.

As far as the depth, yes, the toolpath wont go "Past" the selected surface geometry. The way i would handle that is to leave all 3 surfaces selected, then use the "Botton of Job" setting withing the feature to stop the toolpath where I want. So if you have a ball and wanted to stop the path at the top outer edge of the ball mill, you could calc that. I also suspect you will then see a difference when selecting "tool center" because the geometry selection allows the toolpath to goo "Past" that endpoint... If not, then that can be presented in the BobCad forum for a proper answer,,,

[BurrMan]

when I post the toolpath I get three G3 moves (X,Y,I, and J) at every Z depth rather than one simple G3 circle (I and J) at each depth..

This will be a great question for them in the other forum. They will understand better the connections with the defined machine, the post processor and feature settings, with the posting engine...

They all come together and I am not up to speed on the current stuff

So just to elaborate, I dont have your "Centurion" machine setup, So I have to switch it to my machine. Then that uses "My" post processor...

So when I post the file after making the changes, I only get "2 G3 Movments" on each Z level pass...

I could speculate that my post processor is set to "breaks arcs greater than 180".... Not sure if that is the element controlling this particular break. There are other factors.

These are the things you can get answers from the BobCad guys. They will know how and why the posting engine is breaking the moves...

[BurrMan]

I also suspect you will then see a difference when selecting "tool center" because the geometry selection allows the toolpath to goo "Past" that endpoint... If not, then that can be presented in the BobCad forum for a proper answer,,,

This is another disregard. I just tested it and thats not what that setting is for.

If you set a ball, just set the depth stop to add the balls depth, with all 3 surfaces selected. This will allow the tool tip to go "Past" where you really want the toolpath to stop, and run the ball to the balls center point.

[BurrMan]

It bothers me that, even with the 0.0001 tolerance that you mentioned, when I post the toolpath I get three G3 moves (X,Y,I, and J) at every Z depth rather than one simple G3 circle (I and J) at each depth.

So take a look in your post processor at this line:

204. Are the g codes (G02 and G03) modal in arc milling? n

I set mine to y and got a single G03 for each z line...

[RamseyRuss]

Thanks again for digging into this so far - I hadn't thought that my post processor file could affect the code that much. I will take a look at the 204 line and see how mine is set.
(I have an older machine with very limited memory, so am sensitive to "excessive" lines of code.)

I watched the video (did you have sound? I didn't hear any) - I see what you were talking about with the blending; smoothing out the transitions. I'll have to think about whether or not I want that

So take a look in your post processor at this line:

204. Are the g codes (G02 and G03) modal in arc milling? n

I set mine to y and got a single G03 for each z line...

[BurrMan]

Thanks again for digging into this so far - I hadn't thought that my post processor file could affect the code that much. I will take a look at the 204 line and see how mine is set.
(I have an older machine with very limited memory, so am sensitive to "excessive" lines of code.)

I watched the video (did you have sound? I didn't hear any) - I see what you were talking about with the blending; smoothing out the transitions. I'll have to think about whether or not I want that

Hey RamseyRuss,
No sound in video. Just a visual representation.

The posting engine in BobCad is influenced greatly by your post processor. Also by your machine definition.

Making sure they are robust and properly setup for you is a key element. Don't be scared to spend a little time looking at those.

[RamseyRuss]

Thanks for the suggestion. Yes, I've made a number of changes to my post in order to add additional parameters in the Wizards - to customize for my CNC controller. The change that you're suggesting only tells the post processor that my controller doesn't consider code G3 to be modal - so the post includes G3 on every "G3" line. Unfortunately, BobCAD still thinks that it needs to use three G3 moves to mill a single circle. Consider the following few lines taken from the post. Milling down a constant diameter hole, it is using three circular moves after every depth change - this just doesn't make sense. I'll just have to give it a try, assuming that the three lines of G3 code produce the desired circular path. At least your help with the tolerance setting gets the path into the smaller diameter section of my part.

G01 Z-.2047
G03 X.0389 Y-.0072 I.0393 J.0046
X.0014 Y.0396 I-.0389 J.0072
X-.0393 Y-.0045 I-.0014 J-.0395
G01 Z-.2147
G03 X.0389 Y-.0072 I.0393 J.0046
X.0014 Y.0396 I-.0389 J.0072
X-.0393 Y-.0045 I-.0014 J-.0395
G01 Z-.2247
G03 X.0389 Y-.0072 I.0393 J.0046
X.0014 Y.0396 I-.0389 J.0072
X-.0393 Y-.0045 I-.0014 J-.0395

[BurrMan]

Thanks for the suggestion. Yes, I've made a number of changes to my post in order to add additional parameters in the Wizards - to customize for my CNC controller. The change that you're suggesting only tells the post processor that my controller doesn't consider code G3 to be modal - so the post includes G3 on every "G3" line. Unfortunately, BobCAD still thinks that it needs to use three G3 moves to mill a single circle. Consider the following few lines taken from the post. Milling down a constant diameter hole, it is using three circular moves after every depth change - this just doesn't make sense. I'll just have to give it a try, assuming that the three lines of G3 code produce the desired circular path. At least your help with the tolerance setting gets the path into the smaller diameter section of my part.

G01 Z-.2047
G03 X.0389 Y-.0072 I.0393 J.0046
X.0014 Y.0396 I-.0389 J.0072
X-.0393 Y-.0045 I-.0014 J-.0395
G01 Z-.2147
G03 X.0389 Y-.0072 I.0393 J.0046
X.0014 Y.0396 I-.0389 J.0072
X-.0393 Y-.0045 I-.0014 J-.0395
G01 Z-.2247
G03 X.0389 Y-.0072 I.0393 J.0046
X.0014 Y.0396 I-.0389 J.0072
X-.0393 Y-.0045 I-.0014 J-.0395

The post change i mentioned was to be SURE it was set to yes, and modal...

So indded, you have 1 G03 output there...

There are a few other arc settings in the post that regard breaking arc segments like you show that can be looked at.

I responded to your post in the BobCad form.

You should post this last post and code there and get some help.... i'll check in from time to time to see if you got a reply....

You might want to create a new topic as it IS different than your original post. That way, all eyes may look!