[tOfOloco]

Just curious if anyone else has ever noticed that when you actually use the REAM toolpath under drill, that it calculates feed rates based on the tool having 1 (ONE) flute. ....this is a design error or I'm just really missing something.

Side note: I don't ever use the ream function anyway since it doesn't have a peck function and sometimes I've gotta ream stuff REALLY deep so a chip clear peck or two is nesc.

Thoughts? Comments?

[TonyW]

Yeah, I've noticed that too. Just yesterday again as a matter of fact. I think it's due to the fact they don't give you an option of specifying number of flutes on tool like they do on end mills, etc. Would be nice if they fixed that. Same with drill dialog. Sometimes I use carbide 3-flute drills, but can't select my number of flutes.

Few other things in tool library as well that would be nice to be fixed. Like any tap you choose has an ineffective length of 4.00". Really? wow Quite a few tools have strange defaults and just takes some editing to get them fixed. Been doing that as I go along, not a big deal. But wow, some of the default numbers they use hehe

[Drew24]

Yeah, I love Bob, but it does have some funny quirks about it. Learning curve I am still going through. Like you said Tony 4" ineffective length is a bit much. Haha. I also wish they had a separate tool designation for face mills. It kinda sucks to have to make a 5 in. O.D . inserted endmill. Haha. Nothing I cant work around though.

[bobcad guy]

I Would Like To Second That, And Third That, We should be Able To Set Our Own Defaults For The Features. I wisH The Last Endmill Picked Was The Default Endmill When You Define The Next Feature. Many Times Its the Same Endmill, Little fixes, little Fixes.

[sparkii22]

Do you indicate your reamer in the spindle before you machine? I'm having problems with collet runout and keeping the ream size on deep holes. Is peck reaming accurate? Also, are you drilling or boring the hole and what are you leaving per side? Does this change the bigger ream hole you need?

[The Engine Guy]

.

Just my 2 cents, I always worked on the "ineffective length" being the number of threads on the tap that were not full depth so would not produce a full depth thread therefore have to be allowed for which is why if the number of "ineffective threads" is not correctly set then you will find that the drilling "effective depth" is wrong and can be too deep.

So a value of 4 means four threads at the thread pitch of the tap not 4 inches

Regards
Rob
:rainfro: :rainfro: :rainfro:

[jrmach]

A Reamer is for "sizing" a hole.If you need to have an accurate location,you need better means than drilling.No need to indicate reamer.It should follow the hole,hence,why no drilling if accuracy is needed.Stick a gage pin in collet and check concentricity.If it is acceptable,reamer is at fault.Depending on depth of hole,reamer can be off quite a bit and still accurately size hole.Once again,reamer is for size,it is not for keeping location or even perpendicularity.If the hole walks,so will the reamer.If the hole is straight and you use a slightly out of whack reamer,or bent one,,the hole will still be straight,although may be some bell mouthing at beginning.Reamers have their place,but boring I use more,for a lot of reasons.
Can you give the hole size,depth,tolerances,and material and how many holes ?

[The Engine Guy]

I Would Like To Second That, And Third That, We should be Able To Set Our Own Defaults For The Features. I wisH The Last Endmill Picked Was The Default Endmill When You Define The Next Feature. Many Times Its the Same Endmill, Little fixes, little Fixes.

If you use the software correctly then you very likely won`t ever have any "default" tools appearing, you should have the correct tool for the feature showing up in the tool area.

Simple example :- If you have say 3 drilling operations to do with 1/2", 1/4" and 1/8" drills if you have a Tool Crib already created and saved with say your 20 most used drills in it all you need to do is import that Tool Crib and start doing your features, at the start of every drill feature you are asked to input the diameter and depth of the hole and whether it is through or blind, choosing a 1/2" diameter at this point will call the 1/2" drill at the tool area and there should be nothing for you to do at this area at all

All about work flow and spending any spare time you may have (Not a lot I know ! !) creating tools, setting up cutting conditions and materials to suit the jobs and tooling you do/have.
I mainly work with MS and 6082 T6 Aluminium, not often I use other materials so it was pretty easy for me to set these areas up in the software, now when I set the material in the CAM tree all tooling I use will have the right speeds/feeds at the tool page, all I need do is double check all is as should be and maybe change a coolant setting

What it means is that once all that effort has been put into setting the software up correctly it will translate into a much improved and way faster production of programs for the machine

So, in summary, instead of spending time reading all the rubbish like this that I post may I respectfully suggest you all get stuck into any/all of the above

Regards
Rob
:rainfro: :rainfro: :rainfro:

[sparkii22]

Hi, I was working on a coupling that was welded to a bent tube. There was already a hole there and I indicated the hole. The coupling was 3"deep. The size in the coupling was .73" and I drilled it out with a Guhring drill to .843". The reamer was a about 3" flute length and .875" was the size. Size of hole was supposed to be .875+/- .001. It ended up being .878 and had to be reworked. Unfortunately I didnt have a floating reamer. I had to use an old collet to hold the reamer. I did indicate the reamer in on the machine. This is what all the more advanced machinists told me to do. I couldnt get it any better than .001 though. I am wondering what I could have done differently to get this to be good. I used a 80 CS then did double the feed and half the speed. Was it the hole there that caused it? my .016 per side cleanup? My having to use a collet? Used light tap oil. any ideas or suggestions?

[jrmach]

Is your entire length at .878 or just part of it ?Is the hole round before and after reaming ? This weld you speak of,where is that and how much of that affects the hole ?The weld could make the metal harder the closer to it.What kind of metal ?If it is cast,machine no oil.Being 3 inches,brings problems of it's own.Being bent will be harder to follow the 3 inch of hole.I would scrutinize the reamer.Some V-Blocks and indicator and micrometer.If it checks out try reaming similar material,but at 3/4 inch thick and see what happens.Maybe you need to diamond hone your reamer to size.Get it working on thinner scrap first,then go for the deep hole,this way you eliminate a bunch of stuff.See if it will cut Delrin to size.The better your drill hole is,the better the reamed hole will be.Make sure you get the chips out as they are cut so you are not re-cutting them.Make sure your part is not heating up the more you cut.Thermal expansion will play havoc on doing precision work.Please don't say you are using an adjustable reamer.And how do you re-work .878 hole ?
One last note,I would do this on manual machine so I could "feel" what is going on as I cut.

[Machineit]

As the reamer starts to enter the hole, it is pushed to one side because of the hardened weld. Then as it gets deeper and is more stabilized in the hole, it takes out the weld and the hole becomes out of size. (or absolutely backwards in the weld is on the bottom) Reamers float even if they are not turning true and will almost never change the hole size.

[sparkii22]

Thank you, This was a first time run where I work and I thought it was odd that they didnt have a solid piece there to begin with. Thats good to know the reamer will be ok if it isnt turning true. The weld was on top and bottom of the coupling all the way around it, attaching it inside a larger tube but the coupling stuck out approx .5 on each end. It was a pain.

[sparkii22]

The entire length was at .878 +/- a few tenths. it was only out of round by a few tenths. Attachment 221922 There was weld all the way around the top and bottom of this coupling. It is regular 1080 or something similar. Thanks for the advice. What is Delrin? What is an adjustable reamer? I never heard of that, sorry I am still am a fairly new machinist. By rework I mean the coupling had to be milled out. as far as I know they plan to put a solid piece in this time. Good point. doing it on the manual mill is very good advice I will bring that up to my coworkers.

[jrmach]

Insert Carbide Boring Bar in a lathe would be my choice with your added information.

[Machineit]

Thank you, This was a first time run where I work and I thought it was odd that they didnt have a solid piece there to begin with. Thats good to know the reamer will be ok if it isnt turning true. The weld was on top and bottom of the coupling all the way around it, attaching it inside a larger tube but the coupling stuck out approx .5 on each end. It was a pain.

Yeah, that is far from an ideal condition. Best would be to mill it out close, then ream. But, with a weld it is still difficult. I may even just machine that to size. Reamers are meant to have a little "meat" to bite into and remove, but in a pinch they will burnish a hole with less.

Mike

[jrmach]

3 inch in length I would worry about straightness of hole along with diameter.If the hole is not straight,tight diameter tolerance will not work.
I don't know what the part is,but it looks to be a good candidate for a sleeve or bushing.

[TonyW]

I find that when I am trying to hold crazy size on a reamer, (Like within .0001 - .0002"), rigid reaming will not always hold size. I invested in a 'floating' reamer holder and it has allowed me to hold much better sizes on some reamers. You may want to look into one for yourself. I have a Kennametal reamer holder but a lot of other companies out there too. Just depends on the tolerance you are trying to hold. Also don't feed a reamer too slow. They like to have a good chipload to keep them cutting size.

Hope this helps a little