Contour For Ball End Mill

[richardsalzman]

On the attached model I have two questions:

1.  I selected the same bodies for both operations but still get an error cannot verify stock that has been transfered.

2. On the bottom portion of this part, I want to use a 1/2" ball endmill (tool #11).   I have only used this with a flow tool path before, and this does not seem to be a fit.  I am not familiar with alot of these 3D paths.  What tool path may work best for this complex shape?

Thanks.... Richard

richardsalzman_0-1770400940660.png

[a.laasW8M6T]

Hi

1. Continue rest machining only works with a single body/component selected, If you select CAM Root in the setup it will now work fine:

alaasW8M6T_0-1770411837241.png

2. You have selected a bunch of stuff for heights in the flow toolpaths which are not needed as flow will only machine the selected surfaces.

By selecting a bottom height you are stopping the tool for fully reaching the surface

alaasW8M6T_1-1770412014206.png

also your stepover is very large:

alaasW8M6T_3-1770412496466.png

Flow doesn't work great here anyway

The contour toolpath will be better.

alaasW8M6T_4-1770412520641.png

You cannot machine the whole area anyway as part of it is undercut as we can see from an accessibility analysis

alaasW8M6T_2-1770412392135.png

You may need to re think your design

See attached file with the Contour toolpath anyway.

[richardsalzman]

Hey Andrew.... Hope all is going well with you.   I am a little confused with the concept of an undercut as my intention was to only machine the area shown in blue below with the ball end.  I don't see where there is an undercut in this area.

richardsalzman_0-1770413407987.png

[a.laasW8M6T]

Hi

The Red piece is wider that the green peice

alaasW8M6T_0-1770413874275.png

[richardsalzman]

Thanks... That makes sense.  I enlarged the top by 10/1000 so the end mill would not hit the major diameter of the 1/4-20 threads.  In reality, even if it does, it probably won't matter at all.  I believe most 1/4-20 threads are closer to .2485 instead of .25 so I will fix that and see how it goes.  Thanks for your helps as always!

Richard

[richardsalzman]

Awesome.  That worked great.   Don't I need to do this with a rough step down and a finer step down to get a reasonably smooth finish?  Just curios, for a 1/2" ball endmill, what kind of step down do you think I need for a smooth finish.  I was looking at my speeds and feeds calculator, and I don't see anything for this application.  Once I determine the step over and step down I plan on doing a traditional calculation.  I was thinking of running the endmill at 8000 or 10,000 rpm.  

Thanks so much for your help... Richard

[a.laasW8M6T]

I think with that tool in brass you wont need to do rough and finish passes.

just go straight to finish from the adaptive.

The stepdown I have in the contour toolpath should give you a pretty good surface finish.

In brass you can go 10krpm easy with a 1/2" tool

[richardsalzman]

I ran the first two operation with no issue.   One question; For the last operation, when I hold this part in a vise, how do I determine the lowest point of the tool path so I can make sure I clear the vise?  There is no heights tab for this tool path.

Richard

richardsalzman_0-1770523951829.png

[a.laasW8M6T]

there's several ways of determining the lowest z height 

• you can check the info tab in simulation 
• you can right click on the toolpath and select toolpath data, inspect the data to see the lowest point 
• my preferred method is typically to look at the tool info in the header of the posted code as that will show the z min for each tool, I have also modified my posts to put put the z min as a comment at the tool change.

[richardsalzman]

Wow... Thanks for the awesome tips!  Now that you point this out... I remember that in Tormach PathPilot, you can click on the tool path and see similar information. 

This is going to be a bit tight... Very little to hold on to.  I did not realize this when I set it up.  Fingers crossed!  Thanks for your help! 

[richardsalzman]

The depth of this part is .25 inches.  For fun I ran the last operation with the part sitting on top of a single parallel on the rear jaw of the vise.  The part is out of registration from front to back.  I'm thinking of making the part .10 taller for more contact with the jaws and running it in soft jaws.

richardsalzman_0-1770595222669.png

richardsalzman_1-1770595275032.png

richardsalzman_0-1770609442738.png

[programming2C78B]

Ra to uInch (you probably want a 32-64)
https://www.harrisonep.com/electropolishing-ra.html#:~:text=Ra%20is%20calculated%20as%20the,measured...

convert it to inches
https://www.unitconverters.net/length/microinch-to-inch.htm

then find your stepover amount here based on that cusp height
https://theoreticalmachinist.com/Surface_Finish_Calc.aspx

programming2C78B_0-1770637958529.png

[lauri_barnhart]

Hello, @richardsalzman,

Did the information provided by @a.laasW8M6T or @programming2C78B help you and answer your question?

If yes, please click on the "Accept Solution" button on the post(s) that solved your problem. This will assist other community users in finding and benefiting from this information.

If not, please do not hesitate to give an update in this thread so all community members receive an update on the progression of your question, and can suggest next steps that may be helpful for you to achieve what you're looking for.

All the best,

Lauri | Community Manager

[richardsalzman]

I got myself a bit confused on something.  When I machined the two small pockets (see below) I realized I could improve upon them and programed a radial stock to leave of -.0015 and axial stock to leave of -.008.  Since I made these changes with stock to leave and did not change the model, I expected to run these by entering MDI command of G52 Y .0015 Z -.008.  When I ran it, the tool path was offset in the positive y direction.  I re-ran it with G52 Y0 and it looks good.  What am I missing.

richardsalzman_0-1770954212536.png

richardsalzman_2-1770954603433.png

20260212_112608.jpg

[programming2C78B]

Why would you change your g52? What do you think this would do? 
If you edit the CAM, you don't change the G54. Your work offset position didnt change, your toolpath did. 

[richardsalzman]

I am a little confused on this one.  If I had changed the model, ie made the pocket deeper, the tool paths would change accordingly since I modified the geometry of the pocket.  All good here.

But I did not modify the model, instead I added a negative stock to leave while machining this pocket.  Using a negative STL enlarged the pocket as show with the pink line below.  

Now, when I machine the part that is fixtured in this pocket, the tool path is based upon the position of this pocket.   The location of this pocket is normally dictated by the model.  BUT, this pocket is no longer the same as the modeled pocket, it is larger and the part moved in the direction of the arrow, so I thought I would have to use G52 to move the tool path in that direction.

I believe you are saying that the pocket got larger, but the part stayed in the same location.  Is this correct?

Richard

richardsalzman_1-1771336899094.png

[programming2C78B · Accepted solution]

The center/location of the pocket feature is in the exact same place as before, but the physical pocket is now just .0015" wider on each side and .008" deeper. Most likely that your CAM setup is still using the same location as well, so no WCS adjustments would be needed here...

think of it this way: youre drilling out an existing .25"x0.25" hole with a .253 drill and going .258 deep. Did the hole location change? No.

You're just being thrown off because youre thinking of this as a rectangle and not a hole/centerline. 



If you programmed it to cut -.005 off the wall, but shift your WCS +.0005 all you've done is offset the line back to its original location but with extra steps.

[richardsalzman]

Thanks for the explanation.  Something didn't seem right to me and I could not see why.   Really appreciate your time and patience!