[totalhack]

Ok so here is what I am sure is probably two dumb beginners questions.

I am making a part out of .500 inch hex stock in 1018 steel.

My question is about depth of cut and width of cut when it comes to milling a circular boss.... As I understand it, during a helix cut my step down is going to be the specified amount in my CAM softeare for each revolution of the cutter around the part. IE, my programmed step down is .025 and it will take one full revolution of the cutter around the part OD to complete. Is this correct?

Also what I am unsure of is what number do I use as my width of cut in GWizard. Im being confused because it is a round cutter with hex part stock. Should my cut width be represented by the measurement of the maximium thickness of the hex to the rough OD of my part (.070) Or should my cut width be represented as distance between the two outer most points on the cutter that are in conact with the stock material (.180)? See picture for visual explanation.

So I guess my overall questions are these.

1. Am I correct in that my step down of .025 happens once for every revolution of the tool around the outside of the part?

2. In this example which measurement should be in the "Cut Width" box in GWizard.

Any help and insight will be greatly appreciated.

Attachment 191242

[whateg01]

I'm not an expert on anything, but my experience with MCamX is that the cut width is just the maximum cut the program will let it take. So, that is determined by the tool, not the part. The final pass will be whatever your part shape is.

Without knowing what GWizard does, I would say, save the G-code and have a look at it. Find the G02 and see what it's doing. I know that some control software doesn't seem to like full circles. It likes it broken up into 2 semi-circles. Or, maybe I've done something wrong in the past. But that's what I've experienced.

I'm sure somebody more knowledgeable will come along and correct me if I'm wrong. Then we'll both learn something!

Dave

[totalhack]

I'm not an expert on anything, but my experience with MCamX is that the cut width is just the maximum cut the program will let it take. So, that is determined by the tool, not the part. The final pass will be whatever your part shape is.

Without knowing what GWizard does, I would say, save the G-code and have a look at it. Find the G02 and see what it's doing. I know that some control software doesn't seem to like full circles. It likes it broken up into 2 semi-circles. Or, maybe I've done something wrong in the past. But that's what I've experienced.

I'm sure somebody more knowledgeable will come along and correct me if I'm wrong. Then we'll both learn something!

Dave

Dave, thanks for taking the time to give me a response. Unfortunately it is not the information I am looking for. I am looking for what measurement I should use in the "Cut Width" box in GWizard which is a speeds and feeds calculator.

I actually just created an account on the GWizard forum, hopefully they will be able to answer my question since it is gwizard specific. Thanks anyway though.

Ray

[LeeWay]

I am new to GW myself, but I think your WOC will be .07". You would probably want at least a .14" end mill to be able to make it in a single pass. The larger the end mill I think, the faster you will be able to go. Of course flute count and type also matter.

[totalhack]

I am new to GW myself, but I think your WOC will be .07". You would probably want at least a .14" end mill to be able to make it in a single pass. The larger the end mill I think, the faster you will be able to go. Of course flute count and type also matter.

Thanks for the input, that is what I thought but I wanted to make sure before I accidentally break anymore tooling.

[Hirudin]

Yeah, 0.07 is the width of that cut at that location.

If the speed/feed that G-Wizard spits out looks too aggressive you could change the parameters in your CAM program to cut that profile with two passes of 0.035 each.

[totalhack]

Yeah, 0.07 is the width of that cut at that location.

If the speed/feed that G-Wizard spits out looks too aggressive you could change the parameters in your CAM program to cut that profile with two passes of 0.035 each.

Thanks for the reply! Actually I am a little concerned about the feed rate that GW is spitting out. It is telling me to perform a helical cut at 89 IPM which just seems very fast. I am hesitant to run at the recommended feed. I was going to cut the speeds and feeds in half. Is that a bad idea?

[LeeWay]

Look at the bottom for the turtle and rabbit. Slow it to the turtle pace and see how they look.

[totalhack]

Look at the bottom for the turtle and rabbit. Slow it to the turtle pace and see how they look.

I currently have GW set to 2.0 on the Turtle/Rabbit slider. I am machining 1018 steel. Using a coated .500 x .032 corner radius end mill GW spits out 3686 rpm and 30.60 ipm. Those "seem safe" but what I am scared of is if I use the Interpolation calculator it adjusts the feed rate to 85 IPM. I helix cut the ODs of the part and I have already used the regular feeds and speeds (non adjusted by the interpolation calculator) with good success. Now that I have discovered the Interpolation calculator I am scared to run at the higher feeds and speeds without breaking a tool. Can anyone tell me if 85 IPM seems too fast?

[LeeWay]

I think it is too fast because it is a skip cut. That is for starters. You really aren't interpolating. Sure, you are using a circular path, but the tool is only engaged a small percentage of time. If it was really interpolating a circular path, then the width of cut would be .5".
Interpolating assumes that the tool is engaged at a WOC of .07" the entire path in your application. In other words, it thinks you have already bored a .36" hole in the center. This is why it is giving such high speeds.
I would actually back it off to about 15 IPM and 2500 RPM and see how it fairs. Increase as needed.

I only use interpolation in GW when I am actually milling out a hole.

[tea hole]

I regularly run good carbide 1/2" ems in 4140 and worse from 3000 to 10000 rpm, no joke, from 80 to 125 IPM in a strait line. Assuming a good setup, fixture and that you're climb milling, let er eat. Google trochoidal milling, or look here: YouTube
Remember this one is running dry. I'm sure they are pushing the limits of the tool and spindle as well, but to my point, 80 someIPM, no worries.

[totalhack]

Thanks everybody for their feedback. I ran some parts yesterday and today and I am getting good results. I am running my helical cuts at 42 IPM with a .157 width of cut. Honestly it seems like I can turn up the speeds and feeds even more but I am going to hold back for now. Now I just need to dial in my thread milling. I think I read somewhere that you calculate thread milling just as you would normal milling. Is this true?

[gibbsman]

The following is from Scientific Cutting Tool Catalogue, hopefully it helps.


It may be necessary to use more radial depth passes than shown on the chart (p.36) when cutting
an unfavorable length-to-diameter ratio, coarse pitches, or hard materials. When cutting a thread with
two passes, cut approximately 65% of the thread on the first pass and 35 percent on the finish pass.
For three passes, use a 50/30/20 ratio. For four passes, use a 40/27/20/13 ratio. The idea is to equalize the
side cutting pressure.
Thread mills can sometimes be used to cut multiple start threads. Call engineering for assistance.
Thread mills can be cut off for shorter thread depths or necked back for deeper thread depths. Call for price and
delivery.
In order to apply the Feed and Speed chart appropriately, it is necessary to understand that machining enters will
apply the feed rate at the centerline of the spindle. It is correct to use a normal calculation and the following Feed
& Speed Chart when cutting in a straight line; however, it is incorrect when cutting an internal thread. Therefore,
the feed rate must be recalculated.
the following is an example of how to apply the feed rate correctly:
The tool is a TM290-24A cutting a 3/8-24 thread in stainless steel.
The outside diameter of the tool is 0.290.
The surface foot per minute (SFM) is 150.
The chip per tooth ia 0.001. The tool has four flutes.
The revolutions per minute (RPM) equal the SFM x 3.82 divided by the outside diameter of the tool.
In this example: (150 x 3.82) / 0.290, which equals 1975 RPM.
The RPM x feed (chip per tooth) x the number of flutes equals the Non-Adjusted Feed Rate or NAFR.
In this example: 1975 x 0.001 x 4 = 7.9 NAFR
The major diameter of the thread is 0.375. We will call this D.
The outside diameter of the tool is 0.290. We will call this d.
We will call the Adjusted Feed Rate the AFR.
The formula for the AFR for internal interpolation is AFR = NAFR x (D-d) ÷ D
In this example: AFR = 7.9 x (0.375 - 0.290) ÷ 0.375
Therefore, the Adjusted Feed Rate equals 1.79. This is the feed rate that will equal 0.001 chip per tooth in the
above example. This is the feed rate that must be used in the CNC program.