"Jagged" Spiral toolpath

[JB7280]

Can anyone help me figure out why this toolpath gets so jagged at the end?  I've cleaned it up quite a bit by playing around with smoothing, in arc filters, but it still causes the machine to vibrate quite a bit at the end.    Fyi, this is not the whole part.  I cut the rest away so I could share the file.  

Thank you.

 

https://drive.google.com/file/d/1vbAHIm2r20hf_NF5BITBQ0Is7ezl0djg/view?usp=sharing

 

[#Rekd™]

I changed the Arc Filter Settings and it seems better (took a while to generate though). Not sure how it will behave on the machine.

[JB7280]

58 minutes ago, #Rekd™ said:

I changed the Arc Filter Settings and it seems better (took a while to generate though). Not sure how it will behave on the machine.

Thanks, I'll give those settings a shot on monday.  At least I was on the right track, with the arc filter settings. 

[ajmer]

take a look at this file

 

ajmer_ihs_SPIRAL.mcam

[bird2010]

Equla Scallop...the step distance will be more even

[JB7280]

16 hours ago, ajmer said:

take a look at this file

 

ajmer_ihs_SPIRAL.mcam 3.5 MB · 4 downloads

Looks like you removed the avoidance, and added a containment.  Is the jagged path stemming from the software trying to avoid that face?

4 hours ago, bird2010 said:

Equla Scallop...the step distance will be more even

That toolpath looks nice.  I'll try it.  Thank you. 

[gcode]

I did this with high speed blend

 

blend.zip

[JB7280]

4 hours ago, gcode said:

I did this with high speed blend

 

blend.zip 539.32 kB · 0 downloads

I'll check that out Monday when I'm back at the shop.   Thank you.   

[crazy^millman]

Can I ask a dumb question here? Why not use a 1/8 stub flute ball endmill if you are worried about rigidity? Use the bull in the floor, but use a smaller tool. Why are you trying to use in essence a size on size tool for such a feature? Back up and approach this differently and you will reduce run time and improve the quality of the work. Really want to be trick get a .375 endmill with a .062R made on it and plunge in one shot dwell after roughing with a .005 smaller tool.

[JB7280]

20 hours ago, crazy^millman said:

Can I ask a dumb question here? Why not use a 1/8 stub flute ball endmill if you are worried about rigidity? Use the bull in the floor, but use a smaller tool. Why are you trying to use in essence a size on size tool for such a feature? Back up and approach this differently and you will reduce run time and improve the quality of the work. Really want to be trick get a .375 endmill with a .062R made on it and plunge in one shot dwell after roughing with a .005 smaller tool.

Really for no other reason than the fact that I didn't want to add another tool just for that one feature.  Also, the feature is inside of a pocket, so there are some limitations regarding reach.  I edited the model, to just leave the feature I was asking a question about.  However, as to your comment about using an essentially on size tool, that is creating a different issue, since I didn't anticipate the "cone" it's leaving on the .251" diameter floor.  So I'll have to do something else. 

 

Garr has a 3.8" endmill with a .060" corner rad, so I think I'll just go that route.    I had thought about that, but we don't get enough money for these parts to warrant a special tool.  Garr having one on the shelf makes it make a whole lot more sense.  

 

Edit - Actually, scratch that.  That's gonna have the same dish on the floor unless I have one made with a flat bottom.  D'oh.

[rgrin]

2 hours ago, JB7280 said:

Really for no other reason than the fact that I didn't want to add another tool just for that one feature.  Also, the feature is inside of a pocket, so there are some limitations regarding reach.  I edited the model, to just leave the feature I was asking a question about.  However, as to your comment about using an essentially on size tool, that is creating a different issue, since I didn't anticipate the "cone" it's leaving on the .251" diameter floor.  So I'll have to do something else. 

 

Garr has a 3.8" endmill with a .060" corner rad, so I think I'll just go that route.    I had thought about that, but we don't get enough money for these parts to warrant a special tool.  Garr having one on the shelf makes it make a whole lot more sense.  

 

Edit - Actually, scratch that.  That's gonna have the same dish on the floor unless I have one made with a flat bottom.  D'oh.

What Crazy was suggesting is to mill the "floor" of that feature with a small tool and then come in with an endmill that has the .062" corner rads and plunge in to finish the walls/corner rads.

 

I assume you're trying to avoid doing that to save a tool change?

[JB7280]

13 minutes ago, rgrin said:

What Crazy was suggesting is to mill the "floor" of that feature with a small tool and then come in with an endmill that has the .062" corner rads and plunge in to finish the walls/corner rads.

 

I assume you're trying to avoid doing that to save a tool change?

Not necessarily a tool change.  Just trying to avoid adding another tool to the magazine, as its almost full and this machine has a bunch of jobs on it that run pretty much constantly.  I ended up just adding a 1/8" ball mill though.

[jstell]

On 4/27/2024 at 5:57 AM, JB7280 said:

Looks like you removed the avoidance, and added a containment.  Is the jagged path stemming from the software trying to avoid that face?

That toolpath looks nice.  I'll try it.  Thank you. 

Yes. That's exactly what's happening.  That's why containment is clean.  I'll have to remember that next time avoidance is giving me messy boundary toolpath.  Sometimes making the avoidance stock-to-leave less than the cut stock-to-leave by a few tenths will help smooth the edge of the toolpath.  But I like the containment.  The other day I used depth limits to get rid of some jerky stuff at the end of a similar toolpath.