chamfering holes

[ibrox2000]

Does anybody have any information for chamfering holes

[Eric S.]

hello

 

You can use a contour toolpath. On the contour parameters page change the contour type in the lower lh corner to chamfer. Is this what you are looking for?

[cadcam]

lets say you want to Spot drill with a 45 deg spot drill and at the same time get the chamfer larger then the hole..

 

When doing the drilling on the second paramater pager were you put the depth you see a little

Calcalter button go there.

 

You will see the tools you need in inside.

[specv]

Autodrill works the best for this one, tell it what you need for chamfer sizes and the spotdrill creates them. also you can use the spotdrill to chamfer larger holes with contour after drilling.

 

Pete

[Rick Damiani]

quote:

---

When doing the drilling on the second paramater pager were you put the depth you see a little

Calcalter button go there.

---

I don't much like the calculator option becasue it adds the calculated value to the depth every time you click it. You get the same results by checking Tip Compinsation, and you can check the value (or add to it by adjusting the 'breakthrough' amount) more easily.

[Steel Surgeon]

lol

 

[ 11-15-2003, 05:23 PM: Message edited by: Newbie ]

[Rekd™]

quote:

---

You get the same results by checking Tip Compinsation, and you can check the value (or add to it by adjusting the 'breakthrough' amount) more easily.

---

As long as you don't mind trigging out the diameter you want by using the depth and angle..

 

'Rekd teh calc rules but needs to save settings better

[Rick Damiani]

quote:

---

As long as you don't mind trigging out the diameter you want by using the depth and angle..

---

With the calculator, you still have to know the finish dia. If you know the finish dia, you can just lie about the size of the tool. Dosn't change the code any.

[Rekd™]

quote:

---

If you know the finish dia, you can just lie about the size of the tool. Dosn't change the code any.

---

I was sitting here reading this thinking; Why would you define a tool dia that is not the dia that you're using to make the part, just to chamfer a hole to a certain diameter..? (Remeber, you can't change the dia value in the Tip Comp dialog, you can only change it using the dreaded calculator or the tools actual dia.)

 

You say it doesn't change the code any, and to some degree you're right, but it affects several things that are better left alone. Including the setup sheets, verify, and many other things that are directly related to the tool's actual diameter.

 

Lets say you have 5 different diameters that you need to create c'sinks for? Are you going create 5 different tools and lie about each of them just to do the spotting and avoid the dreaded calculator?

 

You might as well not use either and just adjust the depth + or - in the Depth box.

 

'Rekd

 

[ 11-16-2003, 12:06 PM: Message edited by: Rekd ]

[david b]

My 2 cents

I use 2d contour chamfer with a ball nose cutter,for larger holes.I think it works great.

 

[Rick Damiani]

Hmmm. Good points, all.

 

I'll have to think on this some more. I don't like the calculator because it dosn't leave a trail I can follow later to try and figure out what I was doing. Yet fabricated tool sizes produce other problems, as you point out.

[Guest CNC Apps Guy 1]

I use the dreaded calculator method too. True it's not tremendously smooth, BUT it gets the job done quite nicely as long as your point/arc is at the top of the surface to be chamfered, and your dool definition is correct. If the tool definition is not correct, all sorts of problems can crop up. JM2C - lying gets you into trouble.

[Eric S.]

If I am just spot drilling the chamfer with a 90 deg. spot drill, I do not use the calculator either. I find it just as easy to just type in the math directly into the spot for the depth.

It is a simple formula for a 90 deg tool.

 

Rad of hole to be chamfered + chamfer size + rad of tools tip= depth of cut

 

this has always worked for me. Also adding a dwell to the cylce makes it look much nicer as well as keepling the chamfer looking consistent.

 

Eric

 

[ 11-17-2003, 11:35 AM: Message edited by: Eric Salsman ]

[d00d]

I use a .900 Inserted carbide countersink then figure 1/2 dia. of modeled chamfer and subtract .050. works like a charm.

[P_Scott]

Rick D.,

 

There is a switch in the "dreaded" calculator that states "Overwrite depth". That switch is just below the one that is defaulted on and says "Add to depth". If you want to change the tool angle simply uncheck the "Use current tool values" switch at the top and then you can put in any angle you have for the tool. HTH

[crazy^millman]

I use the old adjust till you hit the nail on the head method. LOL but serouiusly I have found wit the ops Liabry this helps since we do alot of the same holes just set the operation to incremetnal and it repeats from there just another way to maybe look at it.

 

Crazy Millman

[Sailing4life]

Use Contour tool pass. At bottom of page Contour type toggle to chamfer. Click on chamfer button and adjust size of chamfer need. For cutter comp use wear so you will have g41 in your program.

After selecting chamfer mill right click on tool icon and make sure tip size the same us you have on your tool.

Good luck. Alex