anafranil online
IPB

Welcome Guest ( Log In | Register )

 
Reply to this topicStart new topic
> Plunge milling in Sprutcam
sanjeev
post Nov 6 2007, 07:09 AM
Post #1


Newbie
*

Group: Members
Posts: 9
Joined: 12-December 07
From: India
Member No.: 79



Hi!
I find that plunge milling is the only option to rough out many parts that we are currently doing which involves deep pockets. The reduction in cycle time is substantial and can be improved further.

I am currently using the pattern holes generation in sprutcam to plot plunge points manually, and have written a small sub program for plunging which includes a retration away from the uncut material after reaching the plunge depth.

However this method of programming is extremely tedious and quite a deterrant to using this efficient milling method.

My question is can we achieve this with any of the existing machining strategies on sprutcam, or is there an add in for this strategy available for sprutcam?
cheers
Sanjeev

Sanjeev Kumar S.R
Managing Director
Camtech CNC Pvt Ltd
Go to the top of the page
 
+Quote Post
Sprut_UK
post Nov 6 2007, 08:16 AM
Post #2


Advanced Member
***

Group: Administrators
Posts: 1,091
Joined: 12-December 07
From: United Kingdom
Member No.: 4



Hi Sanjeev, I do not know of another way of doing this in SprutCAM.
I have asked for this operation (plunge roughing) to be added to SprutCAM some time ago.....it might be worth you sending an e-mail to them directly to ask for the function too wink.gif

Can you please explain your method that you use so that others using SprutCAM can give it a try too?
I found this article which explains some of the theory behind the plunge roughing technique: http://www.mmsonline.com/articles/070701.html

Dave

Beer makes you feel how you ought to feel without beer.
Go to the top of the page
 
+Quote Post
sanjeev
post Nov 6 2007, 11:16 AM
Post #3


Newbie
*

Group: Members
Posts: 9
Joined: 12-December 07
From: India
Member No.: 79



HI Dave,
The method I use is pretty straight forward. I usually obtain the boundaries of the pocket or outer contour by either projecting them from a solid model or by 2D geometry creation. Then using 2D geometry creation I create the circle of the same diameter as my cutter. Using debug mode, I try to obtain an approximate location which will form the extreme points in the pocket (e.g four corners for a square pocket). These are the boundary points. I then use the hole making operation and create holes using the pattern option to cover the pocket entirely. An easy method is to roughly create more holes to cover the pocket and then delete the unwanted holes. I specify the DX and DY increments as per the recommendation given by the tool manufacturer. Choose an appropriate hole for starting and spiral mill a hole of slightly bigger size than the cutter. While running the operation, I use "by list" instead of "optimal". This ensures that the cutter does not plunge into solid material directly. Post process the program, to get the hole co-ords and then run a small sub program at those points. This sub program is essentially a drilling sub program with a small retraction at the bottom of the hole in a direction away from the stock(0.5mm) in both the XY direction and z direction, to protect the cutter on retraction.

I hope I have made it sound as simple as it actually is! The time savings is phenomenal! All I have to do ultimately is take a finishing pass on the walls to complete the pocket and remove unwanted corner radius. To give an idea, a step over of 8mm using a 32mm dia cutter gives me a cusp of only 0.5mm which is a breeze for any cutter.

Cheers
Sanjeev

Sanjeev Kumar S.R
Managing Director
Camtech CNC Pvt Ltd
Go to the top of the page
 
+Quote Post
Sprut_UK
post Nov 6 2007, 01:23 PM
Post #4


Advanced Member
***

Group: Administrators
Posts: 1,091
Joined: 12-December 07
From: United Kingdom
Member No.: 4



Thanks Sanjeev, that is very useful. I do have two questions about this:

1/ Are you using this routine for machining flat bottomed cavities or for an 3D shape?

2/ The retraction move that you use at the bottom of the hole....do you only do this on the second and subsequent rows of holes? How do you determine the direction of retraction as this will alter depending on the direction that the holes are processed and also when the edge(s) of the pocket is reached?

Sorry, that is more than two questions biggrin.gif

Dave

Beer makes you feel how you ought to feel without beer.
Go to the top of the page
 
+Quote Post
sanjeev
post Nov 7 2007, 07:26 AM
Post #5


Newbie
*

Group: Members
Posts: 9
Joined: 12-December 07
From: India
Member No.: 79



Hi Dave,
Right now I have used this only for flat bottomed pockets. Calculating drill depth is a pain in 3D shapes. I wonder if setting the deeper drill depth and restricting the model will help arrive at the correct drill depth....this is something i have not tried yet.

YOu are absolutely right about the direction of the retraction. It changes for each pass. For this I manually change the retraction direction in the sub program. One more way we do it is to have different subprograms with different directions of retraction and call them accordingly.

I am trying to develop a subprogram, that will take in to consideration the increment direction in X and Y and provide the correct retraction. I am working out the algorithm for this. It will take some time. Will send you the sub program once I have it prepared. We use sinumerik 810D so the possibility of developing the sub program exists, and we are working on it.

Plane milling takes parallel passes in XY plane. If we could change the XY plane to XZ or YZ plane it might be possible to develop a plunge milling operation. I am just guessing, the guys at sprut will know this best. I found that Sprutcam 2007 does not offer this operation either. I believe this operation is absolutely essential in these times of squeezed delivery deadlines and margins.
The feed rates achieved in this method is upto 400mm per minute, which is really great!
Cheers
Sanjeev


Sanjeev Kumar S.R
Managing Director
Camtech CNC Pvt Ltd
Go to the top of the page
 
+Quote Post
Sprut_UK
post Nov 7 2007, 11:28 AM
Post #6


Advanced Member
***

Group: Administrators
Posts: 1,091
Joined: 12-December 07
From: United Kingdom
Member No.: 4



Hi Sanjeev, thanks for the info. I have heard and read a lot about plunge roughing, but never actually used it.

I have just tried creating a drilling pattern over a 3D model and SprutCAM adjusts the depth for each hole based on the underlying model........this should make it possible to try your 2D approach on a 3D part.
Is the retract move absolutely necessary, or could a rapid out move be used?

Dave

Beer makes you feel how you ought to feel without beer.
Go to the top of the page
 
+Quote Post
BOB1974
post Feb 28 2008, 09:15 PM
Post #7


Member
**

Group: Members
Posts: 10
Joined: 28-February 08
From: Bournemouth
Member No.: 2,308



QUOTE (Sprut_UK @ Nov 7 2007, 11:28 AM) *
Hi Sanjeev, thanks for the info. I have heard and read a lot about plunge roughing, but never actually used it.

I have just tried creating a drilling pattern over a 3D model and SprutCAM adjusts the depth for each hole based on the underlying model........this should make it possible to try your 2D approach on a 3D part.
Is the retract move absolutely necessary, or could a rapid out move be used?

Dave

Beer makes you feel how you ought to feel without beer.



Hi Dave, Hi Sanjeev,

I've programmed quite a bit on Mazaks plunge milling, both as a circular milling option giving the hole diameter as the cutter size so it plunges straight in and rapids straight out and also as a manual milling op with the 3 axis retract as Sanjeev says.

I honestly don't feel the need for the 3 axis retraction in the roughing stage. So long as the swarf evacuation is adequate that it doesn't drag it up the side of the job on retraction.

The majority of plunging was done in stainless with an air blast. Slightly smaller step-over at 5mm but the feedrate was slightly higher. Off the top of my head with a 25mm 2 tip cutter in stainless - 3300rpm, air blast, 1350mm/min. Straight in and rapid out.

The cusps were larger too but profiling with the same cutter afterwards again, with increased feeds, was better for the tool and tip life.

I'll have a quick look in Sprutcam tomorrow to see if there is an easy way of reproducing the plunge milling the way I do it.

Oh by the way Sanjeev...If you're basically helical milling "spiral mill a hole of slightly bigger size than the cutter" then is there a need for 3 axis retracion at all?

Just a thought.

Good luck with those deadlines :-)

Go to the top of the page
 
+Quote Post

Reply to this topicStart new topic
1 User(s) are reading this topic (1 Guests and 0 Anonymous Users)
0 Members:

 



Lo-Fi Version Time is now: 22nd July 2019 - 10:11 AM