Trimming surfaces

[Jeff the haas_guy]

OK. I got it to work just by clicking on a containment boundry.

[Ocean Lacky™]

Yes, containment boundaries are an important and useful tools in surface machining. The two extra circles are containment boundaries for the toolpaths I ran on your part. I don't know if you can see them. I have Mill3, here.

[Jeff the haas_guy]

Yes, I see them.

 

When the part is done, I will post a picture.

 

Thanks for your help.

 

Jeff

[Ocean Lacky™]

Any time. What kind of work does your shop do? We do forge dies.

[Jeff the haas_guy]

We make wire winding machines for electric motors.

[Jeff the haas_guy]

Im having a problem with finish on this part I wonder if I could get some help with.

I ran a surface finish scallop on this part with .006 stepsover. .500 coated carbide ball endmill, on A2 tool steel. I am getting small flats on the 1.0 radius and would like to know if this is normal or can I get a better finish?

 

Jeff

[Ocean Lacky™]

sounds like you're getting facets, like on a diamond? try a smaller cut tolerance. I usually run somewhere in the area of .0002 or less

[Jeff the haas_guy]

Does that produce a very long program?

[Jeff the haas_guy]

Is cut tolerance, total tolerance, or sharp corner tolerance?

 

Jeff

[Ocean Lacky™]

On the Finish Scallop Parameters page, click the Total Tolerance Button, set Filter Ratio at 1:1 to start. Set Cut Tol. to .0002, Filter Tol. to .0002. Check the boxes to create arcs in all three planes. One way filtering may or may not help you....depends on your machine.

 

The Filter Ratios 2:1 and 3:1 will produce increasingly smaller programs, but the accuracy will decline slightly, as well.

 

I'm pretty sure that's how it all works, hopefully someone with more knowledge will set me straight if I'm too far wrong! HTH

[Müřlıń®]

quote:

---

We do forge dies.

 

--------------------

We've finally discovered the 20th Century.

---

lol welcome aboard....I do forging dies as well...

 

Mastercam is the best CAD-CAM for forging dies....and pretty much everything else

 

 

Hey Haas.....do a scallop on the dish and a paralell on the bevels...

[Ocean Lacky™]

Thanx, Murlin

[Jeff the haas_guy]

Mr Ocean:

 

I ran that program today with the .0002 cut tolerance. It stopped cutting at the top of a cut. The error message said something about the I, J, and K, cant remember exactly how it was phrased. I looked at the program and it seemed to go halfway around the top radius and then went to a G1 code, not finishing the radius. The other program I made did not have this problem. Have you ever had this problem.

 

Jeff

[Ocean Lacky™]

Mr haas_guy,

 

I've seen that error on occaision, not exactly sure why it happens. It's not anything serious(at least in my experiences)....I just block skip and continue....I,J & K are vector coordinates for calculating Arcs in 3d. It's just one of those little things that we 3d surface programmers have to deal with from time to time. I must say that I've not seen one since I switched over to version X. They were sporadic at best in V9, and it happened in all of the surface toolpaths. If it really bugs you....LOL....try adjusting your stepover slightly....from .006 to .0059 or .0061 for example.

 

 

HTH

[Jeff the haas_guy]

quote:

If it really bugs you....LOL

 

And you find that funny, why?

 

Just kidding. I adjusted the program to 2:1 but have not run it yet. I will try again tomorrow. I ran it once, but want to get a better finish before running the REAL parts.

 

Thanks for all your help.

 

Jeff

[Randy Maynard]

Hi Haas_Guy,

 

Surface, Finish, Scallop is a non-planar toolpath. I would not create arcs in any plane. So, use filter, 1:1 is ok, one-way filter is good (should be default but is not), but do not create arcs. It will cause the plane errors (IJK) you are getting at the machine.

[Jeff the haas_guy]

Thanks Randy

[Ocean Lacky™]

Randy,

 

Interesting! How does not creating Arcs affect program size? Just Wondering. I use the Scallop toolpath on nearly every job, I find that if I don't create arcs, I get so many lines of code to move a small distance, that the control can't keep up. 100ipm program feed is lucky to achieve 20ipm actual feed in some cases.....

[Jeff the haas_guy]

Ocean

 

I noticed that the other program I had at 100imp made very shaky moves and I had to slow it down to reduce the vibration.

 

You notice this?

[Ocean Lacky™]

only if I don't Arc Filter. i have some jobs where I'll run up to 150 ipm and ecept for the spindle whine (12000 rpm), you can hardly tell the machine is on.

[Jeff the haas_guy]

I will try it both ways.

 

Thanks

[Jeff the haas_guy]

The arc filter is in the total tolerance menu, right?

 

So I should click all the arc boxes?

 

Do you turn on one way filtering and why?

[Ocean Lacky™]

Right. I won't say you "should", but it works for me. According to what I read in the Help File, One Way Filtering is beneficial for "Some" Machines, and in certain cases, leaving the box unchecked can cause the small flat spots similar to what you were describin earlier. There is not a lot of detail on the subject in the help file, so I don't have a better answer, sorry.

[Jeff the haas_guy]

Thats Ok. You have been a great help.

 

Got to sleep now so I can go to work.

 

Jeff

[Ocean Lacky™]

Jeff, My pleasure. Just trying to pay back a little for all the great things I've learned by reading in the forum....

 

 

Have a Great day tomorrow!