What's new
What's new

How do I avoid nicks around tabs?

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
...other than not using tabs an using a completely different approach.

These parts are motor mounts for an internal project, so the nicks don't really matter. I'm just trying to figure out how to prevent them for when the outer surface finish actually does matter.

Any secret techniques out there? One thought was to take a skim cut rather than a full width cut to the wall.

Thanks.

IMG_4866 (Medium).jpg

IMG_4872 (Medium).jpg
 
We do a similar technique for some parts.

What we do is step down
1/8" or .200 around the whole perimeter to size then cut the tabs with a neck relieved endmill usually 1/4" diameter.

The tabs we just plunge and move around the profile making sure there are enough tabs to support it.

Sent from my Pixel 3 using Tapatalk
 
Ah, so your solution is that the last 0.025 or so of the profile cut is done with a neck relieved tool...so no nicks so long as you only go up/down 0.025 (or whatever the tab thickness might be. Interesting. I've never used neck-relieved tools. Must get some. What else are they generally used for? How much of a relief do they generally have?
 
Are the tabs 2d or 3d? For me 2d tabs leave a witness mark where the machine stops 2d motion to raise then stop again to drop down but 3d tabs the machine doesn't stop it ramps up then down and the tab looks like a pyramid.
 
Ah, so your solution is that the last 0.025 or so of the profile cut is done with a neck relieved tool...so no nicks so long as you only go up/down 0.025 (or whatever the tab thickness might be. Interesting. I've never used neck-relieved tools. Must get some. What else are they generally used for? How much of a relief do they generally have?
We neck them in house on the tool grinder but you can use a spindex and surface grinder. Just need 0.01 or so clearance is all.

We also use thicker tabs. Bump your tab up to .05-.07. they come off easy with a sand pad.

e47c905f99ece593355bd88d1f5061fe.jpg


Sent from my Pixel 3 using Tapatalk
 
I would skip the vises completely for that.

Put 4 little pieces of barstock under where the parts will be.

Align the openings in the parts with a t-slot or holes in your subplate (for tricky stuff align/offset the part origin with slot/bolt hole so you know bolt will fit)

Hold material with a couple toe clamps.

Mill internal features.

M00

Insert bolts/studs/washers, etc.

Slot out part
 
First thing, you are plunging and retracting right on your finish wall. That is
a big reason you are getting those ugly ass gouges. Small lead in/out so you are
plunging/retracting off the wall.

If you are plunging on the finish wall, and you are only getting this gouging in
some quadrants, it probably because your head is out of square.

Make sure that your pre-tabbing finish is a good finish cut. By that I mean, its
right where its going to be, as in a spring pass wouldn't take off any more material.

You can make your tab generating finish cut a few thou out off the finish wall, and
leave a little tiny step.. A little finish work.. But sometimes that's easier.

One thing I've done when its a pile of parts and I want them to look good. And this
takes a bit of hand coding. In my Cam, I'll break up my lines and/or arcs a bit.
Then I can go in to my G-Code and edit in some ramps for a final final finish pass.

Say 1" tall part, Zzero on top. Running straight in the Y from Y0 to Y8.
Already finished down to z-.9 or -.95 or something.

G0 (or 1) Z-1.02
G1 Y1.
y1.1 Z-.97
Y1.3
Y1.4Z-1.02
y4.
y4.1Z-.97
y4.3
y4.4y-1.02
y7.
y7.1z-.97
y7.3
y7.4Z-1.02
y.....

Ramp length, and tab thickness and width is up to you.
 
A spring pass over the top of your tabs will help.

If your careful you can get away with only ONE tab. Rough and finish your part with 0.100 or so left on bottom to hold it. Then you can plunge in full depth and go all the way around and stop just short of where you started. I do this all the time. You need to pay attention to the stock remaining outside the part, always need solid stock holding the part. Never finish off your single tab on a thin section next to vice jaw. Try it, it works great for quick and dirty jobs not worth doing a fixture for.
 
That's some pretty bad gouging (not nicks). You either have an out of square head, or really bad runout at the Tool. Or shitty Tool holding. That's probably the worst non-accidental gouging I've ever seen.

Were it me, I would start with runout at the Tool, then check movement in the holder. Then move on to the Spindle head.

R
 
That's some pretty bad gouging (not nicks). You either have an out of square head, or really bad runout at the Tool. Or shitty Tool holding. That's probably the worst non-accidental gouging I've ever seen.

Were it me, I would start with runout at the Tool, then check movement in the holder. Then move on to the Spindle head.

R

its a hass cutting thats why, there too sloppy so you have to be way lighter on the finish passes and give them a a dry pass or too. Im guessing a vf2ss or smaller.
 
Im guessing a vf2ss

Correct.

No issues with head out of tram or runout. The machine makes beautiful parts, clean and square. I just don't do this tab thing very often, so I'm sure I'm screwing it up.

I ran another set of parts. This time I did a 0.010 finishing pass. Better. I have some ideas based on the various comments here. I might make a simple test part just to try out a few options.

One thing nobody mentioned (other than one person suggesting the tabs could be thicker than 0.025) is vibration/resonance of the part itself causing a no-win situation. After all, the walls along one axis are fairly thin (1/8) and the tabs are 0.025. Hard to say what that combination amounts to in terms of part rigidity.

The other thought I had is that spacing the tabs equally and symmetrically might also be a mistake. This is how you encourage resonance, which isn't a good thing at all when you are machining.


Also, I'm using CAMworks, which means that a lot of things take a ton of work. I mean, I get carpal tunnel just from the excessive clicking around you have to do. I've been wanting to move away from this thing since I got it back in 2008 or thereabouts. Considering HSMxpress (which I've already installed into Solidworks for testing). I've been paying CAMworks thousands of dollars per year for maintenance for over a decade. Their database still sucks and they want many more thousands for high speed machining...I'm done. If I am going to be aggravated by a CAM tool at least let it be free.

It's the year 2020. I have a 32 core machine with a massive amount of memory, multiple GPU's and ridiculously fast everything...and these tools are still as dumb as a brick.

Sorry for the rant.
 
It's not the machine. It's the fact it's in California [emoji23] blame it on the crying liberals stomping around or even an earthquake.

Sent from my Pixel 3 using Tapatalk
 
That's some pretty bad gouging (not nicks). You either have an out of square head, or really bad runout at the Tool. Or shitty Tool holding. That's probably the worst non-accidental gouging I've ever seen.

I had another look at the picture. I think I understand what you are talking about. The major gouging you see on there is my super-skillful cutting of the tabs with a Milwaukee vibrating blade tool and then taking a file to the thing to clean-up the mess I left behind with the vibro-matic. I just had to get the thing done.

The nicks I am referring to are the thin vertical lines that correspond to the start and end of each tab. The rest is my "artistry".

Sorry for the confusion.
 
its a hass cutting thats why, there too sloppy so you have to be way lighter on the finish passes and give them a a dry pass or too. Im guessing a vf2ss or smaller.

It has nothing to do with being a Haas, unless the machine is beat to shit. We regularly run little parts / tools (parts .5x1x1 for example, and endmills and drills down to .006") and we don't have any of this...

I imagine its partial programming error (no lead ins as Bob said), work holding, etc. The machine will do what you program it to do, right or wrong. Is the machine new enough to have G187? On the tabs, after making sure you have a lead in-lead out, you could add something like G187 P3 E.002/.003 or so...

edit: we check our parts using microwave/ frequency readings... last part I did .0003" comp on a finish tool (1/32") changed the frequency/bandwidth or whatever it is by something like 200Mhz *I think*... I don't have much to do with the lab, I just adjust the parts as needed. :)

edit 2: the reduced shank endmills look like this https://www.mscdirect.com/product/details/61726667
thats' a ball end, but if you look, it is a 1/2" endmill (cutting diamter) with a 7/16" shank. Available from almost anyone, MSC is just easy to find. There is a member here (probably a few) that sells, search around and you will find them...
 
It has nothing to do with being a Haas, unless the machine is beat to shit. We regularly run little parts / tools (parts .5x1x1 for example, and endmills and drills down to .006") and we don't have any of this...

I imagine its partial programming error (no lead ins as Bob said), work holding, etc. The machine will do what you program it to do, right or wrong. Is the machine new enough to have G187? On the tabs, after making sure you have a lead in-lead out, you could add something like G187 P3 E.002/.003 or so...

edit: we check our parts using microwave/ frequency readings... last part I did .0003" comp on a finish tool (1/32") changed the frequency/bandwidth or whatever it is by something like 200Mhz *I think*... I don't have much to do with the lab, I just adjust the parts as needed. :)

edit 2: the reduced shank endmills look like this https://www.mscdirect.com/product/details/61726667
thats' a ball end, but if you look, it is a 1/2" endmill (cutting diamter) with a 7/16" shank. Available from almost anyone, MSC is just easy to find. There is a member here (probably a few) that sells, search around and you will find them...

Mike
I have a hass also I run everyday on small parts. vf2ss machine will make those marks unless you finesse the program.
Those marks are cause by inexperience and the smaller hass machines.
if he ran the finish passed 1-2 times as a dry pass they wouldnt be noticed even close to what they are now.
My fadal with the semi bad spindle makes those marks if I dont program for it(2 dry pass's). My fadal with the good spindle does not.
Those marks are caused by tool load and rigidity of the machine.
 
I had another look at the picture. I think I understand what you are talking about. The major gouging you see on there is my super-skillful cutting of the tabs with a Milwaukee vibrating blade tool and then taking a file to the thing to clean-up the mess I left behind with the vibro-matic. I just had to get the thing done.

The nicks I am referring to are the thin vertical lines that correspond to the start and end of each tab. The rest is my "artistry".

Sorry for the confusion.

Just so we're on the same page the marks that are circled? Correct?

20200429_092455.jpg
 
Just so we're on the same page the marks that are circled? Correct?

View attachment 286709

Yes. That's it.

Someone else just posted that they have experience with this on a VF2 and that it is due to inexperience (guilty as charged), machine/tool rigidity and tool loading.

That said, I am becoming convinced that there's also an element of the part vibrating during the cut. This would be easy to prove by just making the tabs much thicker, like 0.250.

I don't want to make more of these parts but I am really thinking about designing a simple part to test various ideas. May it can be as simple as a 1/2 in tall rectangle, 1/2 in by 2 in plan view with a few tabs around. In other words, make it thick and wide enough that part flexibility isn't as much of an issue as it is with 1/8 thin walls.

I have to go to Industrial Metal today or tomorrow. I usually load-up on off-cuts for experiments when I go there. Trouble is they are not allowing entry into the store because we are all potentially radioactive. I don't have any material I can waste for this experiment right now.

Thanks for the input.
 
Or do it another way.

Start with a little bit thicker material, hold on the extra material. if your part is 7/8" thick, use 1" hold on .1

Machine your ID, OD, face and chamfers. ID can go through and OD should be a hair deeper...

Flip your part. locate a feature for zero, then face off to size, chamfer and you're done. No need to play around with tabs, slug falling...wedging. No deep profiling that has you double cutting chips. No finishing ops to clean up the sides.

I can machine pretty aggressive only holding on 1/16...
 
Mike
I have a hass also I run everyday on small parts. vf2ss machine will make those marks unless you finesse the program.
Those marks are cause by inexperience and the smaller hass machines.
if he ran the finish passed 1-2 times as a dry pass they wouldnt be noticed even close to what they are now.
My fadal with the semi bad spindle makes those marks if I dont program for it(2 dry pass's). My fadal with the good spindle does not.
Those marks are caused by tool load and rigidity of the machine.

It's not "because it's a Haas". Do you really think those tabs are more rigid than the machine? GTFOH
 








 
Back
Top