Coolant or not

[BenK]

I'm running a .625 SGS V-carb in 1045 using a dynamic path. The tool is getting really hot and the corners are not holding up but the chips look good and the part is staying cool. Would you try using coolant or do you think that would shock the tool too much.

[Dave.L]

I'm running a .625 SGS V-carb in 1045 using a dynamic path. The tool is getting really hot and the corners are not holding up but the chips look good and the part is staying cool. Would you try using coolant or do you think that would shock the tool too much.

 

 

Here we go, the war on coolant vs. dry....your gonna get evey opinion you can imagine. I am a huge fan of coolant and always will be.

[Mr. M]

Coolant! Through the spindle would be best!

[EX-wccprogrammer]

Coolant here also. The more, the better. Run flood AND thru-tool if possible.

[Tim Johnson]

Ok I'll be the first For 1045 keep it dry. If your tool is getting hot you're probably not pushing it hard enough. If you can't push it harder then cut the rpm a little. Make sure you're getting two colors in the chip.

[BenK]

I'm going 4200 rpm @ 100ipm 10% step over 1.6 deep. The chips are two colored.

[Reko]

The tool is getting really hot and the corners are not holding up but the chips look good and the part is staying cool.

 

When you say, "the corners are not holding up," are you using a Bull EM with a radius? That would be my suggestion. Go to a bigger corner radius... say, .060"

 

If that EM is anything like a Z-Carb, run it dry, and +1 to the slow the RPM's.

 

S3270 F36. is where I would be on low carbon steel.

[Goldorak]

i use air blow

 

the temperature get more stable than with coolant

[Reko]

i use air blow

 

the temperature get more stable than with coolant

 

Yes. That too.

[Newbeeee™]

We run a 17-4ph job a couple of years ago and had the oportunity of running seco V sandvik inserts.

Wet made the inserts last twice as long as dry, no matter what we did.

[peon]

Air blow and increase the chipload till you get a blue chip in 1045. You're not pushing that tool hard enough.

[MIL-TFP-41]

no coolant....air blow. Step up your feed to 140 IPM & leave the RPM where you are at. At 100 IPM with a 10% stepover your chip is too thin....or wait....I think the V-Carb is a 5 fluter....so maybe 178 IPM

[BenK]

Yes it is a 5 flute. I was running air.

[Tim Johnson]

no coolant....air blow. Step up your feed to 140 IPM & leave the RPM where you are at. At 100 IPM with a 10% stepover your chip is too thin....or wait....I think the V-Carb is a 5 fluter....so maybe 178 IPM

 

The HEM calculator set at 350sfm is S4278 @ F178.27 (11.14CIM). With not knowing your part or machine you could also try a 5% engagement to cool down your end mill, S5348 @ F460.09 (14.38 CIM).

 

The chip needs to have enough mass to be able to absorb the heat created from the cutting. If the chip is too small then the excess heat will move to the next path of least resistance (usually the end mill).

[BenK]

Machine is a Makino A77 50 taper

[AshM]

slight change of topic,

 

What types of toolholders are you all using? I've been using ER40 collet chucks for almost of my machining including the dynamic paths...

[rgollar]

I always use er-32 on size collets this makes a big difference and the shortest holder possible. I also make sure to indicate the end mill and make sure its running true withing a few tenths at the most. And yes cut much faster and keep the rpm the same. I also run dry and when running at them speeds you really dont need air as my machine gets a good cleaning when im cutting like this. Its sprays chips like a power washer. I would start out at 175ipm but I really think you will end up around 230 ipm esp. with five flutes. Just watch for cutting in corners with five flutes and they can become clogged quick but not usually with a 10% step over. I cut that all the time with rpms of 4600 and feed rates of 200 plus with 10% percent step over with no air or coolant. I have had one end mill last for over 100 parts with no problem and was amazed. Now your machines plays a big part in this because if you dont have high speed machining then no matter what feed rate you use the path gets to many points it will not reach the feed rate.

I have seen this to many times I tell people I cut them speeds all the time with no problems. Then I go and see them try it and there machine bogs down to 20% of there feed rate in areas. Then cant figure out why there having problems. So that is another thing to keep in mind. Wish I had a 50 taper to play with. That could really speed things up with that rigitity. Oh on that note make sure you set up is solid because if there is any vibrations due to lack of solid set up you can hang it up. Hope I did not ramble to much and good luck.

[BenK]

I'm us Albrecht milling chucks for any path like this. the setup is rigid. I always watch to see if the machine is reaching the feedrate, with the size and shape of this part it wouldn't have a problem with reaching any feedrate. Thanks for all the feed back, I'm going to take this too my meeting next week so keep the suggestions coming.

[rgollar]

well I would say your using a good chuck. I think im going to get one myself as I have always thought the er series limited me alot. Now I have to find me a vendor in my area or call there site. Thanks

[MrFish]

The Z-carb is ti al coated is it not ? so the hotter it gets the harder the coating gets (to a limit) so the heat shouldn't be too much of an issue , if you can i'd use MQL for cooling and lubrication to reduce the chip friction. Also i would check the run out of the cutter if you are only using ER collets as it could be loading up one cnr at a time causing the failure.

[BenK]

The Z-carb is ti al coated is it not ?

 

Yes that is the coating on both the Z-Carb and V-Carb.

 

only using ER collets

 

I'm us Albrecht milling chucks for any path like this.

[Joe788]

Ben, could you just try coolant and see what the difference is? I think your chipload is way low, and bouncing it up to JMC's suggestion will probably solve most of the heat issue. Not sure if your corners are crumbling because of heat though. I use dynamic and optirough in 17-4H1150 dry, and get pretty good tool life.

 

 

Edit to add: Do you know there's another guy on the forum who works at K&G?

[BenK]

Edit to add: Do you know there's another guy on the forum who works at K&G?

 

Yes I do, thats how I got this job.

[cincy k]

Not to thread jack but what is a HEM calculator?

[Tim Johnson]

The HEM calculator is an Excel file designed to calculate speed/feeds for dynamic/peel type milling thet was created by Terry from Iscar primarily for their Chatterfree end mills. The file is in the tools folder on the FTP under HEM Calculator-protected.xls (also .ods).