Help with milling cast

[JacobRuter87]

I am new to machining (>15 months). I am trying to machine out some older Minneapolis Moline heads and I have been having a bear of a time. I have broken a 7/8" & 1" roughing endmill. I have also had the collet come loose 3 times on me. It was a brand new tool holder and collet, so the first time it happened I just figured there might have been a bur or something that was stuck in there. I am climb cutting (that is what I have been told is the best way to do it, per school instructor/former machinist). I know some of the issue I have been fighting is I have to have to tool hanging out a ways because I have to go 5.25" deep in some spots. Other spots I can go 3" from each side and I don't have these issues. I am really out of ideas and am hoping someone more experienced than me could offer some advice, because I am running out of ideas and booze to help with the headaches this thing is giving me.

 

[edwards.a]

Unfortunately I don't have a lot of experience with machining castings, but I can ask some questions that will help someone else help you better:

What kind of machine are you using for this operation? Manual? CNC?

What kind of speeds and feeds are you using?

What is your depth of cut and stepover?

What kind of tool holder and collet are you using? Do you have access to different toolholders? I will say I generally avoid using collets for endmills that large.

What kind of tools are you using? Are they Ebay/Amazon endmills or from a reputable brand ?

Could you rough out material using a shorter stickout tool and finish with the longer stickout?

 

[JacobRuter87]

Unfortunately I don't have a lot of experience with machining castings, but I can ask some questions that will help someone else help you better:

What kind of machine are you using for this operation? Manual? CNC?

What kind of speeds and feeds are you using?

What is your depth of cut and stepover?

What kind of tool holder and collet are you using? Do you have access to different toolholders? I will say I generally avoid using collets for endmills that large.

What kind of tools are you using? Are they Ebay/Amazon endmills or from a reputable brand ?

Could you rough out material using a shorter stickout tool and finish with the longer stickout?

Working on a Haas CNC

300 RPM 2.0 Feed rate

.125" depth of cut. No real step over. The center was water jetted out and I'm coming back through and cleaning up to finished size.

I am using an ER 40 collet, both are Accupro, we don't have a different holder for a 1" tool

Tools and holders all come from MSC but the 2 endmills that broke are there value brand

I roughed the first step with a 7/8" and went down to 3 1/2" depth and then used the longer 1" to go the next 1.75" deep and that is were I am having issues with the collet coming loose.

 

[edwards.a]

So again I don't have experience with cast iron at all and also have more experience with lathes than mills, so take my advice with a grain of salt. But until someone else chimes in....

Are you using carbide endmills? I'm assuming you are using high speed steel based on that rpm. If my calculations are correct that is about 78 sfm for a 1" endmill. Never used high speed steel so I don't know if that is right or not, but the tool supplier/the internet should be able to tell you. My iscar book recommends approximately 300 sfm for a carbide endmill.

Feed rate seems slow but again I don't know this application. Also, it is important to specify the number of flutes on the endmill as the important consideration is generally feed per tooth.

I'm also a bit confused about what you mean by ".125" depth of cut. No real step over."

Are you doing the cut in one pass? How much material are you taking off? Perhaps I wasn't clear in what I am asking, this link should help with any confusion:

Optimize Depth of Cut and Stepover for Better CNC Milling

Optimize Depth of Cut and Stepover for Better CNC Milling Note: This is Lesson 5 of our Free Email Feeds & Speeds Master Class. Click

www.cnccookbook.com

See: "Defining Depth of Cut and Cut Width"

 

[JacobRuter87]

So again I don't have experience with cast iron at all and also have more experience with lathes than mills, so take my advice with a grain of salt. But until someone else chimes in....

Are you using carbide endmills? I'm assuming you are using high speed steel based on that rpm. If my calculations are correct that is about 78 sfm for a 1" endmill. Never used high speed steel so I don't know if that is right or not, but the tool supplier/the internet should be able to tell you. My iscar book recommends approximately 300 sfm for a carbide endmill.

Feed rate seems slow but again I don't know this application. Also, it is important to specify the number of flutes on the endmill as the important consideration is generally feed per tooth.

I'm also a bit confused about what you mean by ".125" depth of cut. No real step over."

Are you doing the cut in one pass? How much material are you taking off? Perhaps I wasn't clear in what I am asking, this link should help with any confusion:

Optimize Depth of Cut and Stepover for Better CNC Milling

Optimize Depth of Cut and Stepover for Better CNC Milling Note: This is Lesson 5 of our Free Email Feeds & Speeds Master Class. Click

www.cnccookbook.com

See: "Defining Depth of Cut and Cut Width

I am doing it in one pass, no step over. .125" depth of cut. It is a cobalt endmill.

 

[mhajicek]

I am doing it in one pass, no step over. .125" depth of cut. It is a cobalt endmill.

I think you misunderstand. The width of the cut is called "stepover", even if you're only making one pass, so if you're taking off .125" in the X/Y plane, that's a .125" stepover.

My first thought is you probably didn't tighten your collet nut hard enough. Those ER-40's take a bit of oomph. Check the recommended torque, and see if you have a torque wrench you can use.

 

[michiganbuck]

Consider the direction of your feed and if when climb milling you might pull the part forward so taking up the clearance in your feed screw, plus the feed rate..

 

[JacobRuter87]

I think you misunderstand. The width of the cut is called "stepover", even if you're only making one pass, so if you're taking off .125" in the X/Y plane, that's a .125" stepover.

My first thought is you probably didn't tighten your collet nut hard enough. Those ER-40's take a bit of oomph. Check the recommended torque, and see if you have a torque wrench you can

Maybe I am just misunderstanding. I am taking .125" for the depth. due to the roughness of the cast in some spots its .8 in the x/y and .3 in others. I am just running a profile around it to clean up from the waterjet. I leaned pretty hard into the wrench when I tightened it but we don't have a way to torque the nut. The last time I got it as tight as I could and then used a plastic dead blow against the end of the wrench to get a little tighter. I got the fist half done. I need to move the clamps so I can get at the second half and hopefully it will stay tight.

 

[Houdini]

How many flutes, does it have a coating on the end mill. need to know how thick the material is you are cutting off?
collet shouldn't come loose, make sure its really tight, but also this may seem like a stupid question, but you are making sure that you are popping the collet up inside the nut,
and assembling the the nut and the collet together before you put them on the holder correct?
but 180 RPM and 2 ipm for a 4 flute.

 

[Houdini]

.3 to .8 WOC ouch, HSMAdvisor says that's too much for a cobalt end mill, tool breakage, you need to break up that width of cut.
really shouldn't do more than 50% diameter, try .25" width of cut.

 

[mhajicek]

^^ What he said. .800" is way too much stepover for that endmill. Take much lighter passes.

 

[Houdini]

if your doing a lot of these and want a super cheap indexable find out who your local ZCC USA supplier is,
it is a cheap Chinese indexable, but more rigid than a cobalt end mill.
ZCC USA 90 deg indexable

 

[???]

You can definitely take full width of cut on a HSS tool with the correct speed and feed it was done all the time. I have also experienced cutters coming loose on a casting. In my case it was a 38mm long series HSS endmill in a Titanic chuck. I changed to side lock and that ended the problems. It's probably a lot cheaper to sort out your tool holding and tooling than mess around for hours breaking cutters.

 

[Houdini]

You can definitely take full width of cut on a HSS tool with the correct speed and feed it was done all the time.

Didn't say you cant, just said you shouldn't.
And relative to the cut at hand, overly long noodle cutter, too much tool engagement.

I have also experienced cutters coming loose on a casting. In my case it was a 38mm long series HSS endmill in a Titanic chuck. I changed to side lock and that ended the problems. It's probably a lot cheaper to sort out your tool holding and tooling than mess around for hours breaking cutters.

100%, a cheaper side lock holder would be better in this scenario fo sho! IMHO

 

[Houdini]

You can definitely take full width of cut on a HSS tool with the correct speed and feed it was done all the time.

You mean like this?

 

[JacobRuter87]

I will cut my step over back to .250" for the thicker parts and will order a side lock holder and hope that works better for the next 2, because it would be a long week machining if stuff doesn't get better. Thank you for all for the help.

 

[Orange Vise]

I know some of the issue I have been fighting is I have to have to tool hanging out a ways because I have to go 5.25" deep in some spots. Other spots I can go 3" from each side and I don't have these issues.

5-6 times the diameter on a cobalt endmill is going to cause serious problems. Cobalt/HSS has less than a third of the rigidity of carbide, and even carbide doesn't play well at those types of stickouts unless you're cutting aluminum and plastics.

What's the absolute largest diameter tool you can get in there? At 5.25" deep, I'd usually go for a 1.5" diameter indexable cutter. It's going to be substantially more rigid than a cobalt endmill because the shank of the indexable is solid, i.e. full 1.5" diameter, whereas the endmill will have a core diameter of roughly 60% of the cutting diameter or ~0.600". Considering the deflection of a cantilevered rod is proportional to the radius to the 4th power, the indexable in this case will be about 30-40x more rigid.

As for the collet coming loose, this is probably due to a combination of insufficient tightening torque and heavy vibration in the cut. We torque our ER40s to 150 foot lbs, about 3X as much as you're going to get using a stubby ER wrench.

 

[Houdini]

5-6 times the diameter on a cobalt endmill is going to cause serious problems. Cobalt/HSS has less than a third of the rigidity of carbide, and even carbide doesn't play well at those types of stickouts unless you're cutting aluminum and plastics.

That's what I said, I would rather run a cheap ($100 with inserts) Chinese index-able than run that cobalt end mill.
@ the low cost just add it to the bill. finish pass still gonna be a good time though with that end mill if a single pass cleanup is needed.
, with the lack of rigidity in a Haas(he didnt say what size)
might need to up the rpm drastically and take a whisper cut to unload the tool and not flex the machine.
I have to do this on my Haas machines with long stick out carbide finish pass end mills even, let alone roughing, I only rough my stuff with a 1.5" index-able actually.

 

[The Dark Bike Co]

A Weldon (set screwed to flats on the endmill) toolholder is really the only way I would hold tools of that size.
And yeah, stepover isn't helping you in any way.