[Helo500]

Tried out V26 and then got the yearly sales call, so if this sounds a bit terse, it is.
There is an ongoing bug in the lathe tool generation back to at least V23. It shows up when trying to use Cutting Arc Center compensation under posting on current settings. The bug is in the tool creation engine in the cam tree. If you create a new tool or modify an existing tool, that tool is now bad. The pointer for the orientation is off by 1. Existing tools in orientations 1 and 5 have their theoretic points for Z and X both negative. Your new tool has a positive Z. If you use only the original tools in a feature, it will generate the correct tool path offset to the outside of your part by the tool nose radius. If you pull in a tool you have created, it will be wrong with the tool path inside your profile in Z. The thing that will drive you nuts is that if you modify anything on the tool in a feature, that part of the software will set the orientation back to the correct Z theoretic offset again in that feature. In versions 23 to 25 you can use this to straighten things out with the tool path. In version 26 the tool creation is still bad, and is carried into the tool crib. But now the toolpath engine seems to create the correct offset in Z for the bad tool, and the wrong offset in Z for the good tool. It seems to ignore the X value altogether.
Told the salesman I would be be happy to explain this to programming. They have my number.
Hopefully Al or Burrman will see this and rattle somebodies cage.

[woffler]

By God you right ,but what to do about it ?

[mmoe]

Told the salesman I would be be happy to explain this to programming. They have my number.

This isn't how it works really. Use the bug reporting portion of the Bobcad website and submit the bug in a thorough and well documented manner. They do look at them and evaluate them carefully to determine if there is indeed a bug, so it's not a waste of time at all.

[BurrMan]

Hopefully Al or Burrman will see this and rattle somebodies cage.

Mentioned in the esteemed realm of Depoalo.... COOL!

I cant really recreate this, but I don't really have a very good understanding of what I should be seeing when I do whatever, on the Turning side.

I would have to ask to go step by step, and have the results pointed out to me that are incorrect. I created a simple sample and moved, added, deleted and modified tools and their parameters, but didn't get any change in the "backwards z/x theoreticals"...

Are you drawing your parts in the negative x, positive y quadrant?

Use the bug reporting portion of the Bobcad website and submit the bug in a thorough and well documented manner.

This is what I do........ But I have to be able to re-create it and understand it before I do that.

Maybe Hood will see this and jump in. I know he's a lathe guy...

[Helo500]

Hi BurrMan,

I posted this issue on the old Bobcad forum several years ago. Programs were uploaded and you pm'd Sean to look at this. It was given a bug number, and was to be fixed.
If you open the lathe tools from the top of the cam tree and look at the Z and X theoretic values for original Bobcad tools, they are both negative for tools in orientation numbers 1 and 5. If you create a new tool here the Z value will now be positive on that tool. These are the values for orientation 2.
These values are used to offset the toolpath from the part, just as the toolpath is offset by the cutter radius when profiling on the mill. This will carry into the tool crib on V26. If you load the tool into a feature, it still will show a positive Z value and will offset the tool path into the part instead of outside it.
If you make any changes to the tool from the feature page, it then will change the Z value back to a negative. The new toolpath will now jump back outside the part. In V23 to V25 you can "shake" the tool in the feature by changing the orientation from 1 to 2, close, reopen and change back to 1. This corrects Z and gets the right path. In short the software pointer for orientation values in the tool creation at the top of the Cam tree is off by 1 position.
In my short look at the V26 demo it seems that a change has been made in the toolpath area that will treat the Z value opposite from previous versions. So now getting the Z theoretic value back to a negative will give the wrong path inside the part. Positive now creates the correct Z offset, but can't be maintained because if you edit anything on the tool within the feature, Z returns to negative. X now seems to be ignored and generates no offset.
Clear as mud, right.

[Helo500]

Hi BurrMan,

Second post to answer your questions.
The profile of the part is in the positive X , negative Z quadrant of the lathe screen. Z 0.0 is the face of the finished part. Cutting arc center is selected under the posting on the current machine settings tab. A cross section of a trailer hitch ball works good for testing. Z axis right through the center line.
A finish pass around this with a cutter that has a .125" nose radius, should have a nice offset path .125" outside the part profile.
The toolpath should look the same as if you laid the profile on the XY plane in mill and profile cut around it with a .25" end mill.
Try it with a tool you created in the cam tree and pull into the feature with no changes. Then go into the feature and "shake" the tool. Rerun the toolpath and see if it changes.
If the toolpath is inside the profile, you just crashed the machine.
A 2.5 pound chunk of Stainless-Aluminum at 3500 rpm exiting the lathe, through the window, tends to upset the operator.

Thanks for looking at this again.

[Hood]

Can you provide a bbcd file so I can see what you are meaning?
I never use the arc centre method personally so not quite clear on the steps.
With regards the orientation again I am a bit unclear as I dont have the option of 5, just 1-4. I have however deleted all standard BobCAD tools and made up my own as BobCAD ones are Imperial and they just get converted to metric if you are set up in metric units and thus they are not quite correct, so much easier just to scrap all the standards and set your own. I think however if you provide a file the tools will be included, so I can look.
For me, tools with Orientation 1 and a 0.8mm nose rad have the X offset -0.8 and z offset 0.8, which seems correct I think.
Hood

[BurrMan]

Thanks for looking at this again.

Hello Helo,

I reported this. With no job tree, I right click on Cam Defaults-tool library-Lathe-Rough-Add.

If I select orientation #2, the theoretical changes. If I change it back to 1, nothing changes.

I also reproduced the "shake the tool" scenario you listed.

Although I don't understand enough about it to walk through where an error is, there is an inconsistency going on.

Let's see what happens.

[Helo500]

Hi Hood
I don't have a file handy, but will see if I can put one together in V25 tonight. The X and Z theoretics for your tools should both be negative in orientation 1. Since you created all of them, they will have the positive Z value. I misspoke on tools 5-8 since they are internal, but they are still off by one when created. The X and Z values are the offsets from tool radius center to the cutter face you are using, represented by the red dot on the tool picture. So for orientation 1 the direction to the cutter contact point is negative in X and negative in Z referenced to the tool radius center point. If you are turning off compensation within Bobcad and simply programming to the part outline, you may not see a problem. I can't use positive offsets in our lathe, from the home position without getting OT alarm, so I must program from arc center with compensation on.
If you bring one of your tools into a feature, change orientation from 1 to 2, close, reopen and change back to 1, does your Z theoretic point return to positive as it came in? Or is the Z value negative as it should be?

[Hood]

Ok just been looking at the offsets and they do seems screwed.
I have not noticed this as I am using System Comp with Collision detection and it seems to programme correctly.

I have just looked at my tools and they all seem wrong now that I look at things.
Orientation 1 - Z pos X neg (think both should be pos)
Orientation 2 - Z pos and X pos (think Z should be Neg)
Orientation 3 - Z neg and X Pos (think both should be Neg)
Orientation 4 - Z neg and X Neg (think Z should be pos)


Its early morning here (2am) so the brain is working at less than its normal 10% so maybe the above "think z/x should be" are not correct but seems right to me
So it does look like they are off in BobCAD.

This may be the reason things are screwed if I choose system comp but without collision detection.

Hood

[Helo500]

Hello Burr,

When you go into the tool creation in the cam tree and look at an unmodified Bobcad tool it will show negative X and negative Z. If you hit add, the template still shows -X and -Z. For V26 change anything on the template besides the tool label.
Close the window and then reopen. Look at original Bobcad tool, it is -X and -Z. Look at the tool you just added. It will be -X and positive Z. This is the value for Orientation 2.
The pointer routine within the software is off by one position.
When I looked at the V26 demo, it looks like the toolpath routine may have been changed to compensate for this bad tool creation. This really messes with things when the feature routine sets the tool back to the right values.

[Helo500]

Hi Hood,

I finally had to open Bobcad and look at the tool orientation to get this right. Memory is not as good as it once was. Orientations 1-4 are turning, 5-8 are facing.
Orientation 1 and 5 - Z neg X neg
Orientation 2 and 6 - Z pos X neg
Orientation 3 and 7 - Z pos X pos ( These last four are the internals I was thinking of.)
Orientation 4 and 8 - Z neg X pos

These are the correct values. These are what you should get if you reorient the tool in a feature and then set it back.

Also noticed that the tool picture in V26 does not change to match the orientation as it did in previous versions. Also the red dot for the theoretic point is actually blue. Oops!


Mike

[BurrMan]

Hello Burr, When you go into the tool creation in the cam tree .

Yes, I saw it. I reported it to BobCad.

I think it's an error in the tool library dialogue. I don't think there are any errors in the toolpath though, like I don't think they are generating toolpath "incorrectly to match the error in the dialogue".... I think it's just an error at creation, then once the error is passed into the system, that's where things get confused and values can be "shaken" by the existing system.

[Helo500]

Hi BurrMan,

I believe it is a very simple bug in the tool creation. Someone started with an array pointer of 1 instead of 0. I'll have to look at V26 demo a bit more , but it looked like action in the toolpath creation is now reversed.

Attached is a file created in V25 showing the effect on toolpath. In this file green path is mostly correct.

Mike

[Hood]

I have just installed Dolphin on this new computer so I can see what it says and it seems to correlate to what I was thinking. I wonder if definitions are specific to the programme or maybe even they are different as Dolphin is calling it offset and BobCAD is calling it theoretical point.
Anyway here are a few pics of each orientation showing both BobCAD and Dolphins offsets.
I will see if my old version of FeatureCAM will work on this comp or maybe see if I can get the demo, and have a look and see what it calls out for these offsets.

BTW sorry for not having the same nose rad in both, just noticed when I looked at the screenshots but it doesnt matter anyway as all we are concerned with is the actual pos or neg.

Hood

[Hood]

Got FeatureCAM demo installed and it looks like it agrees with the way Helo500 is saying BobCAD SHOULD be saying. So looks like Dolphin is indeed looking at the actual offset rather than the programmed point.
Anyway here is what FeatureCAM shows which is the exact opposite of Dolphin but I think what is agreed that BobCAD should be showing?
Hood

[Helo500]

Hi Hood,

The actual values can be positive or negative depending on which way you reference them. It doesn't matter as long as the toolpath engine is setup to use them correctly.
Bobcads original tools were correct. It is only the tool creation routine in the top of the Cam tree that gets things wrong. The editing routine used in the feature for tools puts it back right again. I'm sure Bobcads programmers can fix this in an hour, once they see it. Problem is it's a sneaky little SOB because it changes back and forth. Took me a long time to figure out what was really going on.

Mike

[Hood]

The thing is that my tools are permanently wrong then. If I add a new tool the orientation is showing as 1 and both offsets are negative. Now that seems to be right from what you are saying. As soon as I change anything, in fact dont even have to change anything, simply click any entry then clicking another will change the Z to a positive value.
So my tools for Orientation 1 are always Z pos, X Neg. The only time I would ever manage to have both negative for Orientation 1 is if I create a tool and change absolutely nothing.

This may explain a few weird things that I see if I dont use the collision detection in turning ops, and do use collision detection in grooving.

Hood

[Hood]

Hi Hood,
The editing routine used in the feature for tools puts it back right again.
Mike

Mike, can you point out what you mean by this? My tools always seem to be wrong as you can see in the screenshots below which are taken from within a feature, first is OD turning, second ID.
Hood

[Helo500]

Hi Hood

There is a work around until they get it fixed. If you reorient or edit the tool in the feature, and then reorient it back, that routine will correct the offset values.
You have too watch it a bit to make sure it takes. That usually works in V23-v25.

Mike