toolpath smoothing

[CristiP]

 can somebody help me with the above post regarding simple revolve part and the wavy surface high speed hybrid toolpath? I attached a mcx 2018 file to that post. I canot run such a toolpath on less expesive machines. What ingredients do I have to add to that toolpath to remove these wavy effect. Thanks

[pullo]

scallop is not a very efficient toolpath in your case , as scallop does not follow the topology of your geometry , it offsets the limiting boundaries and  this offseting usually has nothing to do with the best way to machine your part . 

So my silver bullet  is usually pencil , unlimited . Arc filtering etc is totally off ,  This toolpath  will need internal radii in the machining area for the toolpath to start to "follow" the natural shape of your part ( along an internal  / external fillet rather than across it fro example ).  But in many cases there are ways to induce the toolpath to follow the topology

of the part.

I think my pic proves my point way better than 7000 words here .    I know that I machined more than you asked for , but as that area near the internal fillet has to be machined anyway ,might as well do it in one go .  
 

 

 

 

 

 

Gracjan

 

 

 

[pullo]

 I tried  hybrid  , but the quality of the toolpath vs pencil leaves much to wish , cyan is pencil , purple is hybrid.

 

[CristiP]

1 hour ago, pullo said:

 I tried  hybrid  , but the quality of the toolpath vs pencil leaves much to wish , cyan is pencil , purple is hybrid.

 

Thanks. I will try pencil to see the results. My part was the one from the below pitures but it's almost the same situation. I'll try and I'll come back with feedback. Thanks again.

[pullo]

Your part (the plate looking part )is even simpler as  an internal radius is inside the machining area. You must remember  to  force the toolpath to be made by applying the right overthickness.

I was not able to induce a toolpath  creation using old school pencil, but high speed pencil with an overthickness of 6 mm gave me a nice toolpath.

 

 

However, since we are talking molds , those "wavy "  cut entrances and exits will make the guy who has to polish this surface curse  you till the end of time.

You need here a toolpath with  one entry and one exit. Here the right choice is High speed spiral, especially since your part is circular.

 

 

 

Gracjan

[CristiP]

27 minutes ago, pullo said:

Your part (the plate looking part )is even simpler as  an internal radius is inside the machining area. You must remember  to  force the toolpath to be made by applying the right overthickness.

I was not able to induce a toolpath  creation using old school pencil, but high speed pencil with an overthickness of 6 mm gave me a nice toolpath.

 

 

However, since we are talking molds , those "wavy "  cut entrances and exits will make the guy who has to polish this surface curse  you till the end of time.

You need here a toolpath with  one entry and one exit. Here the right choice is High speed spiral, especially since your part is circular.

 

 

 

Gracjan

I've tried with pencil but still "wavy". I have just drive surfaces, a boundary and an overthickness of 6mm. Can you give me your mcx file please? 

 

[CristiP]

15 minutes ago, Help_me said:

I've tried with pencil but still "wavy". I have just drive surfaces, a boundary and an overthickness of 6mm. Can you give me your mcx file please? 

 

It seems that if I change the tolerance a little, thing are getting better. The above picture was calculated with a tolerance of 0.025 and a stock to leave zero. If a leave a stock of 0.01mm on the surface it is ok, no "wavy" toolpath. The trick here is to play a little with the stock to leave and the tolerance I think. For example If I left zero stock on the surface and a tolerance of 0.025 no chance......but if I change the tolerance for example 0.06 I avoid the "wavy" toolpath.

 

[pullo]

Pencil unlimited would be in my opinion a general solution for creating smooth toolpaths in complex  topography. But since your example here is circular ,  it's definitely  spiral the way to go  in my opinion . 

 I would not  classify my toolpaths  into good/bad just by looking from the side , unless you have some problems with achieving  a good finish by minimizing the change in your Z 

axis.  Do you have Heidehain in your machine for control ? 

GRacjan

  

[CristiP]

3 minutes ago, pullo said:

Pencil unlimited would be in my opinion a general solution for creating smooth toolpaths in complex  topography. But since your example here is circular ,  it's definitely  spiral the way to go  in my opinion . 

 I would not  classify my toolpaths  into good/bad just by looking from the side , unless you have some problems with achieving  a good finish by minimizing the change in your Z 

axis.  Do you have Heidehain in your machine for control ? 

GRacjan

  

I agree the spiral it's more suitable for this part but I'm not looking for the best toolpath to make this part. It was just an example to show you those waves or Z changes along the toolpath. I have hermle C32U with heidenhain TNC640 but here there is no problem with these Z changes along the toolpath but on less expensive machines the surface finish and tool movements are serriosly affected by these kind of toolpaths. For those machines I use powermill because there I did not see these Z changes along the toolpath. I will practice more with stock to leave and tolerance to obtain a more smooth toolpath with less Z changes. Did you try it with 0.025 tolerance and stock to leave zero and then same tolerance but stock to leave 0.01?  I'm not classify my toolpaths from the side view, but if this is a problem in making your machines to not work properly or to affect your surface quality...Thanks

[pullo]

OK , so you have one of the best machines , so Z is not a problem .  So I  would go with Spiral , total tolerance 0.004   ,  for D8R4 a step of 0.12 will give you a miiror finish.

For your other machines , if you want to maintain a constant Z, thereby allowing for the creation of arcs  in your NC-code , I woukld suggest the classic Contour , with shallow turned on.....

 

 

 

[CristiP]

2 minutes ago, pullo said:

OK , so you have one of the best machines , so Z is not a problem .  So I  would go with Spiral , total tolerance 0.004   ,  for D8R4 a step of 0.12 will give you a miiror finish.

For your other machines , if you want to maintain a constant Z, thereby allowing for the creation of arcs  in your NC-code , I woukld suggest the classic Contour , with shallow turned on.....

 

 

 

I agree. I'll try contour also with shallow turned on. Thank you very much for your help. 

[Müřlıń®]

Same hybrid tool path with a solid instead of a surface....

No fancy filtering....

Learn what makes the software tick and you will stop going in circles...

 

 

 

 

[CristiP]

2 hours ago, Müřlıń® said:

Same hybrid tool path with a solid instead of a surface....

No fancy filtering....

Learn what makes the software tick and you will stop going in circles...

 

 

 

 

ok, but you have only 4 drive surfaces and you need 5 in order to machine all the cavity. You did not select the outer most surface, the yellow one from the below picture. If I do the same the toolpath is also ok like in your picture, but if you select a boundary and you choose stay inside -0.2 to keep the tool like in the below position you will see that your results are different.

[Guest]

I offset it a different way but I dunno, looks reasonable to me

 

https://www.dropbox.com/s/uaqop82kfh5f8y0/JP_heavy and wavy.mcam?dl=0

[Müřlıń®]

 

Are you saying you don"t want to roll around the outer wall and want to start the tool at .75?

It's easily done with modified geometry to keep the solid trimmed edge at the correct depth so the cordial error doesn't get multiplied a million times when you choose it as

a boundary.

 

[CristiP]

1 hour ago, JParis said:

I offset it a different way but I dunno, looks reasonable to me

 

https://www.dropbox.com/s/uaqop82kfh5f8y0/JP_heavy and wavy.mcam?dl=0

thank you : ) looks good! 

[pullo]

I also made a solid .  I also know that Mastercam internally breaks solids into surfaces,  so working on a solid is not the silver bullet here.  

The bar was set here to output as much constant Z  as possible .  You can get Hybrid to look constant Z from a distance , but the ultimate test is how many arcs form in the NC-code. The file JP provided ( the one which looked best  to me of all the hybrids  I tried ) formed a few arcs at  the center of the part and  on the outer shapes  so in a 11 000 line program we get some arcs until line 280 , then  it's lines and a fluctuation in Z . 

I played around with the JP hybrid  to maximize the number of arc I  got (i.e.. a measure of true constant Z ) and here are the results :

JP used a step of 0.29 and I got a program of 8500 lines  (heidenhain code , so an arc takes two lines), there were 143 arcs in the code

A constant Z  old school program with flat turned on in order to be somewhat comparable to hybrid created  1600 lines of code and there were 567 arcs in the program.

Only  arcs are displayed in the following pics :

 

I am done with this subject . 

Gracjan 

 

 

 

[Müřlıń®]

"  so working on a solid is not the silver bullet here."

 

It is the solid chain that gets rid of the waviness...

I showed several examples. in other posts where using boundary chains created off surfaces that had large cordial deviations

would translate back into the tool path and produce those...

The initial post was to get rid of the waves not tell him the best tool path to use or create a tool path with the most arcs..

We do 5-Axis tool paths that have almost no arcs that produce a mirror-like surface finish.

I get irritated when people don't know how to use the software come in here and say "Mastercam can't do it I will just use Powermill"

 

[huskermcdoogle]

7 hours ago, Müřlıń® said:

I get irritated when people don't know how to use the software come in here and say "Mastercam can't do it I will just use Powermill"

Yeah that has always bugged me as well.  But what frustrates me as a mastercam user is how to gain the understanding how to do things sometimes.  I have a problem I have dealt with for ages that I thought I had licked the other day.  Turns out, I don't and am still figting it.  I have to make a sample file and post it up.  My luck I will make the file and it won't do what I struggle with..... 

[gcode]

8 hours ago, Müřlıń® said:

It is the solid chain that gets rid of the waviness...

I've had good luck smoothing things out with the

"Projected boundary smoothing tolerance" on the Toolpath Control page

[pullo]

I think this one is flogged to death : ) . 

Gracjan

[pullo]

As usual , we almost went off topic.  The topic was  "toolpath smoothing" .

I think we can all agree that ,  when creating a toolpath that does not seem to be  doing it's job , 

all the smoothing in the world won't  correct the situation .  Everybody ditched the idea of applying some magical smoothing parameters and went off on a tangent with this or 

that idea.  Correct me if I'm wrong.... 

As to the Powermill thingy , there's  at least 250 000  of us . 

Gracjan

[jlw™]

I personally would create a little geo, revolve a surface and use flowline set to spiral with gap setting bigger than my step over and "follow surface."  that will be a smooth path foshizzy.

[pullo]

yep , proved my  point ))))

Gracjan

[gcode]

On ‎6‎/‎14‎/‎2018 at 8:08 AM, LucasGC said:

for the operation or in my mcam settings?

GB1-3920-10-00.mcam

I am unable to work with this file

It opens OK, but says my Sim is not enabled for this product

My personal sim is current and includes the full suite of multiaxis toolpaths

I'm guessing the machine/post is protected.

I tried changing to a generic 5X machine but it won't let me do that either