Not getting a correct tool path!!!!!

[RStuart]

Okay, I am machining a pocket roughly 6 inches in diameter, .625 deep with a full radius in the bottom. This is something that is pretty easy and we have been doing for some time now with no problems. Now all of the sudden when I do it, it looks fine in mastercam but when machined the finish contour toolpath is not acurate. It leaves a good finish on one side of the part and a choppy finish on the other. Almost acts as if the arcs are off at each depth but only on half the part. Why is this and what can I do to fix it?

[RStuart]

I have uploaded a file in the MC9 folder on the FTP site named stu.mc9

[RStuart]

I am running this on an okuma mill.

[RStuart]

The toolpath seems to be breaking a perfect arc into two seperate arcs and one arc is the good toolpath one is the bad toolpath. The 2 arc have different radii and different center points. Why. The geometry used to create the surface was a circle.

[Fig sign]

RStuart!

Try this :

1.Tighter your filter settings ten times. total tolerance 0.0002

2.Change tool containment to center .

I tested with this settings and I satisfied with results

HTH

[lynnz]

RStuart,

I agree with Iskander. Tighten up filter tolerance. I usually rough with .002" total, then change total to .001" or less on finish.

Although why with your current settings would 1 side be smooth and other side rough??

 

Lynnz

[lynnz]

RStuart,

I agree with Iskander. Tighten up filter tolerance. I usually rough with .002" total, then change total to .001" or less on finish.

Although why with your current settings would 1 side be smooth and other side rough??

 

Lynnz

[RStuart]

I have tried tightening my tolerances and it does no good. Or am I defeating the purpose by filtering the nc in nc utilities?

[Fig sign]

quote:

---

Although why with your current settings would 1 side be smooth and other side rough??

---

When your geo . created it has it`s own tolerance .

Create your curve for check boundariies using create->curve with not tight const.param and it can close your surface a bit .

And with check boundaries settings inside it can lead to the mentioned above result.

That`s why I changed it to center

HTH

[Fig sign]

~~~~~~~~~~~~~~~~~

filtering the nc in nc utilitie

~~~~~~~~~~~~~~~~~~~~~~~

Avoid using this sort of filtering ,it is not associative and lacks some other things .Use filtering inside your operation ,tighten tolerances ,check in one way filtering and set check boundaries to center .

 

HTH

[RStuart]

I am creating these surfaces by first creating a solid then changing it into a surface then deleting the top surface. Is this creating a problem? Never has before.

[Fig sign]

Rstuart !

 

Just tighten the tolerances and all the other stuff and run a test .

~~~~~~~~~~~~~~~~~

It leaves a good finish on one side of the part and a choppy finish on the other

~~~~~~~~~~~~~~~~~~~~~~~

This can be the table backlash

Iskander teh never mind

[lynnz]

RStuart,

try going to Modify-Normal-Set-All-Surfaces.

I did this to your file and the normals reversed on 3 surfaces. (all of them)

It may make a difference. If this was a solid with the top surface removed, the normal is on the outside.

 

lynnz

[RStuart]

Okay, I have tightened all the tolerances as suggested above, 99.9% sure it is not the machine and still am not getting the correct tool path. Why is it breaking up the arc section into two arcs with each arc having a different center point. I think this is where my problem is. Again it is finishing the left side of the part well but the right side is choppy and not smooth, does not follow the contour! Any other ideas?

[RStuart]

I am still trying to figure out why I am not getting a good tool path on this. Any help guys?

[Fig sign]

Too busy to help now .

Sorry

[Fig sign]

Rstuart .

I really very busy.

But 2 words .

Filtering is always approximation .

If it is too deviating from your tolerance tighten filter settings .

Not enough -tighten more !

Read in Mastercam help about filtering and you`ll understand what I mean and what to expect .

You call your toolpath choppy ?

Save your tolpath through backplot on the separate level ,build surfase section (slice ) on the same depth as a toolpath and compare (measure deviation ) .it will be in your toleraned limits !

So is it really so critical to lick your program days?

Run it ,and give to the quality check !

I bet it will pass it .

 

 

Teh

[P_Scott]

RStuart,

 

I've looked at your toolpath and posted it out using the post you had selected from the list of generic posts available to me. I don't believe it's actually anything to do with the toolpath itself. I've produced a picture of the code as it is backplotted from Cimco Edit Pro. The name of the pic is "stu_mc9_nc.bmp" and can be found in the MC9 folder on the forum FTP (side note to Jay aka Cadcam - please place picture in this thread if possible). The blue entities in the pic indicate arcs in the code. The Filter settings are working in the toolpath. I didn't do anything to your settings. Because of the tolerances in the post for outputting arcs as "R" instead of "IJK", there would end up being a slight difference in the center point location. The actual difference between the "R" values of each arc is between 0.0003 to 0.0005". That's not a lot. There happens to be a larger difference between the center points however. Try changing the output of your arcs to IJK instead of R and see if that helps to clean up your toolpath. Another option would be to use an alternative toolpath, like Surface-Finish-Project-Blend and use the top boundary as the first chain and a point in the center of your part as the second boundary chain. HTH

[cadcam]

As asked for by Peter Scott,

[Code_Breaker]

quote:

---

Avoid using this sort of filtering ,it is not associative and lacks some other things. Use filtering inside your operation

---

Iskander, when using toolpath "3D Swept", the option to filter in the toom Manager is greyed out and not available. The only way to filter the toolpath is NC Utilities. Agreed that the file is not associative, but what are the other precautions? Just plain curious.

 

 

Code_Breaker

[Fig sign]

Swept will produce clean toolpath from clean geometry ,it is always clean ,cause it not accepts splines

No need to filter it !

[Code_Breaker]

quote:

---

Swept will produce clean toolpath from clean geometry

---

Yes, but it is point-to-point. Unfortunitely, our machine hate the code. So, I filter it in NC Utilities to give me code with arcs.

 

I know you'll say, "get a new machine", but it is not in the budget. Everytime it brought up, the owner stop the conversation, "end of discussion!"

 

So, I am left with producing the best type of output for our machines.

 

Code_Breaker

[P_Scott]

Thanks Jay!! "You Da Man"!!