cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Chamfer diameters and drill depths

Newbie

Chamfer diameters and drill depths

I have been doing holes in parts for years and they always have to be tweeked at the machine tool. Pro gets in the ballpark but not accurate. I am building my tools as assemblies and I want to make my tools accurate. What are the options to get want I want? I am currently using a standard drilling sequence for spotting and setting a blind, tip hole dapth and I use a make datum thru on all my other drilling. I am trying Csink but it is not comming out accurate either.
5 REPLIES 5
Highlighted

Chamfer diameters and drill depths

Terry,

As far as c-sink dia's are concerned, I always put a dwell in for that
cycle (G82). It really depends on how fast you are feeding. I would
start maybe with a .5 sec dwell. Depending on the controller the depth
may vary, even the 'z' depth is correct.
Hope this helps

Tony



On May 3, 2010, at 4:55 PM, Terry Thomas <->
wrote:

> I have been doing holes in parts for years and they always have to
> be tweeked at the machine tool. Pro gets in the ballpark but not
> accurate. I am building my tools as assemblies and I want to make my
> tools accurate. What are the options to get want I want? I am
> currently using a standard drilling sequence for spotting and
> setting a blind, tip hole dapth and I use a make datum thru on all
> my other drilling. I am trying Csink but it is not comming out
> accurate either.
> Site Links: View post online View mailing list online Send new
> post via email Unsubscribe from this mailling list Manage your
> subscription
>
> Use of this email content is governed by the terms of service at:
>

RE: Chamfer diameters and drill depths

I have a few areas that I am seeing issues for drilling/ countersink accuracy. I need to centerdrill some holes in a part that I am working on. I have a chamfer that is the same angle for the centerdrill that I am using. If I use the countersink type sequence the tool works on the chamfer angle but comes up shallow. If I use standard drill sequence the tool stops at the end of the pilot drill diameter. I also have built all my tools as assemblies and the assemblies also do not work correctly. I need to adjust the drill point to compensate for the flat on the end of the drill as well.

Chamfer diameters and drill depths

Terry,



For spot-drilling/countersinking purposes we use tool types
"COUNTERSINK" or "DRILLING". We use both parameter (xml) tool files and
solid tool models. There is a parameter named "POINT_DIAMETER" that you
can fine-tune to match the web thickness of your actual tool. Without
setting this parameter correctly, you will always end up too deep
because the depth will be driven by a theoretically sharp pointed tool.




For center drilling, we use tool type "CENTER_DRILLING". However, this
does not have a parameter for the point diameter, so you need to fudge
some other parameter such as pilot length to make theory match reality.



For toolpath creation, we use HOLEMAKING, COUNTERSINK for all of the
above. "Auto Chamfer" is handy if every hole has chamfers modeled and
the chamfer angle of the tool matches.



Finally, G-Post does not natively support converting CL "CSINK" cycles
to machine software cycles. We have FIL routines to convert the CSINK
cycles to "DRILL" cycles and process accordingly.



Regards,

Dave Ford
NC Programming Mgr.
G.W. Lisk Co.
Clifton Springs, NY 14432
(315) 462-4381



P Please consider the environment before printing this email - be green,
keep it on the screen!


Chamfer diameters and drill depths

Terry,

We have recently worked through this same issue. What we've basically
determined is that Pro/E is perfectly accurate when the actual tool
geometry matches what Pro/E thinks you're using. In the case of an
insertable chamfer mill, the difficulty arises because the cutting edge
of the tool does not lie on a plane extending through the tool's axis of
rotation (at least not on the type we use). Simply giving the tool a
point diameter to compensate is not accurate either because the point
diameter value (effectively a z-offset) needs to changed based on the
diameter of countersink. The closer the hole/countersink size is to the
thickness of the insert, the larger the point diameter value needs to
be. What this also means is that a tool like this doesn't truly cut a
flat surface as it rotates. The surface will actually have a slight arc
to it, and this arc will increase greatly near the tip of the tool.

In an attempt to find a way to accurately compensate the tool at
multiple diameters, I modeled up the tool's insert in Pro/E and then
also modeled up what Pro/NC thinks its cutting. The difference is
fascinating. After a couple of different approaches I was able to
finally realize that a couple of triangles can easily represent how the
tool will actually behave at any cutter depth. After playing with the
math a little bit I was able to come up with two formulas. One formula
takes the target diameter and returns the actual depth. The second
formula takes the cutter depth and returns the actual diameter. Here
they are:

Actual Diameter = ( ( SQRT( ( Insert Thickness / 2 )^2 + ( TAN ( Insert
Angle / 2 ) * Target Depth )^2 ) ) * 2 )

Actual Depth = ( ( SQRT ( ( Target Diameter / 2 )^2 - ( Insert Thickness
/ 2 )^2 ) ) / TAN ( Insert Angle / 2 ) )

(spaces for readability)

- Insert thickness is the total thickness of the insert and assumes that
half this value extends beyond the plane thru the center axis
- Insert angle is the angle the insert has on it, not the angle of the
wall it cuts. For a 90 degree mill, use 90. For an 82 degree mill, use
82.

Right now I'm not actually using the second formula for anything. Here
is how I am using the results from the first formula in Pro/NC:

1.) Set point diameter to "0" or "-" in the tool definition
2.) Create a drilling sequence with a blind depth in the hole set
3.) Create feature level relations to read the tool diameter and
point angle and then calculate how deep to really go.
4.) Use feature level relations to set the z depth of the sequence.

That makes it sound complicated. It's really not bad at all. Here are
the actual feature level relations from one of my counter sinking
sequences. Note: the logic to read the starting hole size (before
counter sinking) is not shown here.

/* CALCULATE COUNTERSINK DIAMETER BASED ON INITIAL HOLE SIZE
CSK_DIA = (HOLE_SIZE + 0.040) /* We use 0.020 per side

/* READ INFORMATION FROM SELECTED TOOL
TOOL_FEED = TOOL_ROUGH_FEED_RATE:TID_CSK_10000_04C2_N:1
TOOL_SPEED = TOOL_ROUGH_SPINDLE_RPM:TID_CSK_10000_04C2_N:1
TOOL_POINT_DIA = POINT_DIAMETER:TID_CSK_10000_04C2_N:1
TOOL_POINT_ANG = POINT_ANGLE:TID_CSK_10000_04C2_N:1

/* CALCULATE REQUIRED TOOL DEPTH
CSK_DEPTH=((SQRT((CSK_DIA/2 )^2-(0.1875/2 )^2))/TAN(TOOL_POINT_ANG/2))

/* ASSIGN CALCULATED DEPTH TO Z-DEPTH DIMENSION OF SEQUENCE HOLE SET
D670 = CSK_DEPTH

/* TIE SEQUENCE PARAMETERS TO TOOL PARAMETERS
CUT_FEED = TOOL_FEED
SPINDLE_SPEED = TOOL_SPEED

Using this logic has allowed us to use our insertable chamfer mills with
complete confidence. No mater what I set for countersink amount or what
hole size is selected (as long as the tool is designed to counter sink
that size hole), the counter sink actually cut by the CNC machine comes
out exactly as intended, every time.

Hope this makes sense, and helps! I've attached a few pictures to this
message that show the type of tool we use as well as a couple of screen
shots from Pro/E of the model I made of the insert.

Tom Uminn
Continental Tooling Concepts
3515 Busch Drive
Grandville, MI 49418

RE: Chamfer diameters and drill depths

It always exciting when I see people using the power of Pro/NC and finding great solutions for problems that exists in every CAM package out there. This solution was very helpful (Using NC-Sequence relations) and this is what Pro/NC is all about.

It´s important to have a positive atitude in regards the software. The name is Pro/Engineer, not Pro/Stupid 😉

My kudos to all you guys!

Daniel

Announcements