2D Compensation - Error

[rafael.sansao]

Hello,

Do you have problems with compensated 2D toolpaths (full radius)?

The NC code return the error on the machine and returns the message "Very large tool radius". (Heidenhain, Siemens, Mazatrol, Fanuc, etc.)

I believe that the problem can occur because the Powermill generates points very close. (Movement of only 0.001mm in X and 0.002mm in Y):

N175X-14.569Y-41.77 *

N180G01X-14.57Y-41772 *

I do not know what else to do to solve this problem. Maybe it's an internal Powermill problem.

can anybody help me? The ideal would be to run the NC on the machine (using any Post-processor)

Attached sample project.

Rafael

[NanchenO]

Hi Rafael,

Did you try with "Point distribution" = "Fit arcs" ?

We have an old Acramatic 950 with a very small memory and use this to reduce the programs' size. Having a look at your model, I think that it will also prevent the programs to have to small lines.

By the way, are you sure that you need a tolerance of 0.01 ? With fit arcs, you will also get less facets than with lines.

Olivier

[rafael.sansao]

Olivier,

I changed the point distribution to "Fit arcs" and the tolerance to 0.02mm.
Still giving machine error.

Check the pictures attached.

Now there is a movement of 0.000421mm in X and 0.0016mm in Y.

Apparently it got worse.

Rafael

[Pijetro]

Do you have any wear values in your offset tables that might be causing the issue?

[rafael.sansao]

Pijetro,

In the table I have the radius set to 8mm and wear as zero.
All right.
The problem seems to be the NC program itself.
Autodesk Developers? any suggestion?

Rafael

[Anonymous]

Hi,

I suppose the problem is that each machine has a tolerance of tool positioning. If the next point of toolpath is in the margin of machine error, it can be impossible to move to that point, that's why machine generate error.

Why won't you use the pattern?

See exapmle below:

https://1drv.ms/v/s!AhIER7BPyy2Xgm5HwA9hsMTmciiA

Mateusz

[NanchenO]

@rafael.sansao,

It seems that your pattern is not 100% smooth. You should normally not have these kind of small moves with this shape.

You could try to activate "Profile smoothing" with a very small value. This should remove these very small moves.

Olivier

[LasseFred]

when i have that problem. i make an arc fit on the pattern, right click on the pattern and then edit click on arc fit seleceted.

in most cases i use 0,02 tolerance on the arcfit,

if this doenset work, i draw my own pattern.

i dont think the 2D feature strategy can´t do what you want.

[rafael.sansao]

@Anonymous

I always use pattern. The example is in Powermill 2017 because Delcam told me earlier this year that this problem would be fixed.

@NanchenO

 Activate "Profile smoothing" does not solve the problem.

@LasseFred

I do exactly the same as you. Do you think a top CAM software should work like this?

It makes no sense to generate an error NC Program on the machine.
This should not be "trial and error"

Autodesk, look at this!

Rafael

[Jaanyaar]

---

piro_man wrote: 

Why won't you use the pattern?

See exapmle below:

https://1drv.ms/v/s!AhIER7BPyy2Xgm5HwA9hsMTmciiA

---

Mateusz, can you please tell me how you created that pattern made of 43 points? I tried to create it by compostie curve command but I would got a pattern with more than 100 points. Insert model command is even worse.

[Anonymous]

Sorry for the trick... It is not the original solid from rafael.sansao file (2D_Machinning.zip). I couldn't open his project because he made it in PowerMill 2017. I have PowerMill 2015. I did the trick and rebuild that solid, but, may by it look's similar, but there are not the same.

Mateusz

[NanchenO]

@rafael.sansao,

In this kind of situations, we extract the curves, open them in the editor, apply a curve fitting with arcs option and the largest possible tolerance and totally forget the surfaces.

When you import surfaces from another software, even if they are actaully cylindrical, they are not always converted into "clean" cylinders. Depending on the conversion tolerance ( too low ), the result could be a very ugly surface ( when you zoom it ). If you try to machine it with a very tight tolerance, then you will get, with the tool's offste, that kind of very short segments that almost no machine can handle properly.

-> Try to extract the curves and have a look at them.

-> If you don't need to be very accurate, try 0.1 tolerance and fit arcs: The shape should be clean, without facets and you will avoid these very small sgments.

Olivier

[rafael.sansao]

@NanchenO

I use these features, however, there are situations that take hours to get a compensated 2d toolpath that does not error.

Sorry, but the CAM software should generate the appropriate path regardless of the situation.

I've worked with various software and never had this problem.

Autodesk needs to look at this.

Case ID: 12332930

Rafael

[NanchenO]

I also used several other CAM softwares and I totally agree with you !

PowerMill is very powerful for complicated things but very heavy to use and unpredictable for simple 2.5 axis machining.

Let's hope that the new 2.5 axis functions will be cleaned up soon, because they are supposed to drastically improve PowerMill's weakness in simple 2.5 D machining. It seems that they definitly need some more debugging to be really helpful in the day to day business !

Olivier 

[Anonymous]

---

@NanchenO wrote:

@rafael.sansao,

In this kind of situations, we extract the curves, open them in the editor, apply a curve fitting with arcs option and the largest possible tolerance and totally forget the surfaces.

---

We move along the same lines as Olivier really.

However, I will say if you can, use tool wear instead. Full radius in confined spaces is unpredictable especially if you play with the diameter of the tool (in the CNC machine control) in order to fit it in.

Some times though I had cases where I had to recreate such curves manually introducing circles myself in PShape in order to avoid situations like these. (Very faceted surface finish etc.)

If you want to extract the profile of a flat surface fast in Pshape there is a command that I have used in one of my old Pshape macros. I could dig this out for you if you want.

Kind regards

George

[NanchenO]

Yes, George, but that's a lot of work for that kind of simple shapes !

PowerMIll's smoothing functionality should be able to do the job without hours of preparation

Olivier

[rafael.sansao]

@NanchenO

Please send me. I want to test

Powermill / Postprocessor should automatically smooth the curve if the 2D compensation is active.

It does not seem so difficult to me.

Employee Autodesk

[NanchenO]

@rafael.sansao,

I wrote that it should... but it actually does not

I sometimes have issues with cutter compensation, but it often comes from a too big difference between theoretical and actual cutter radius.

I also had issues with toolpathes similar with yours, with too small segments. In these cases, I had to do the same ob as George: time consuming and trial and error -> this should be improved !

If I give 0.02 mm tolerance, don't tell me that there is no way to smooth the toolpath in order to avoid  having segments shorter than 0.02

Olivier

[rafael.sansao]

Autodesk is on a group vacation? Funny no employee comment on this!

[rafael.sansao]

up