CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
July 16, 2018, 19:25:25 pm


Login with username, password and session length


Pages: [1]
  Print  
Author Topic: [42] SOLVED - Pocket next step down.. rapids are missing  (Read 3639 times)
Unknownpro
CNC Ewok
*
Offline Offline

Posts: 4


View Profile
« on: May 24, 2016, 23:57:59 pm »

When I choose a pocket and tell it to cut a pass and the pocket is larger than the bit, it makes a slim pass then steps over but once it finished the pass, it slowly moved back to the plunge location.

Can I change the speed where it moved back to the plunge location?

I understand how change the step over speed,  but where is this setting?
« Last Edit: July 07, 2018, 01:50:51 am by dh42 » Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7559



View Profile
« Reply #1 on: May 25, 2016, 00:10:41 am »

Unknown,
Please supply us with a .cb file ( down in "additional options").


We can deal with _almost_ ANY PROBLEMS (no... not all... but 'almost' <G>) if you only supply the source file with which you're having trouble!

LLoyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Unknownpro
CNC Ewok
*
Offline Offline

Posts: 4


View Profile
« Reply #2 on: May 25, 2016, 01:49:04 am »

This is not the actual cb file i am having problems with, but all my drawings have this problem.

so as you can see in the example i have a .6 diameter circle and i am cutting with a 5/16 cutter. it starts in the center then moves to the outer wall, once it finishes the outer pass it then moves back to the center (not pickup/move and plunge) to take the next plunge. it just moves back to the starting point but the move back speed it not the same as the stepover speed.

if you need the real file let me know but its a gun part and i was trying not to post the code online for others to use.

* temp file.cb (3.23 KB - downloaded 80 times.)
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7559



View Profile
« Reply #3 on: May 25, 2016, 02:08:11 am »

First of all, the VERY LAST feed-rate used in that file is the highest rate (12ipm... kinda slow...)... but it NEVER slows down during any horizontal moves, always going at 12ipm

Second, you have a fundamental flaw in your design:  you go to a depth of 0.1.  Depths are ALWAYS negative of zero... zero being the surface of the stock, and positive being ABOVE the stock, while negative is below it.

Last... having corrected that one issue, I see nothing wrong with the code, except that 12IPM is VERY slow... and might be causing what you think you see.

For certain, it only moves slowly while plunging, NOT while cutting...

LLoyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Unknownpro
CNC Ewok
*
Offline Offline

Posts: 4


View Profile
« Reply #4 on: May 25, 2016, 02:30:50 am »

I will give it a try by changing the depth to a negative, however it has never gave me problems before unless I use the surface height. Which then I indicate the - depth.

As for speed it works for me. I am cutting stainless at .04 per pass on a hobby machine.

If I have time tomorrow I'll take the sample file and make a video of the issue and post it on youtube so you can see what I am talking about.

When I mean slow move back to plunge area, like 2ipm speed slow. Not sure what mach3 says as for the speed,  never looked at the read out.

Thanks. For your help.
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7559



View Profile
« Reply #5 on: May 25, 2016, 02:56:12 am »

"I will give it a try by changing the depth to a negative, however it has never gave me problems before unless I use the surface height. Which then I indicate the - depth."
-----------------------
I do not care what 'problems' it has created... it is incorrect.  It WILL create problems later, when you have both positive and negative depths in complex designs.

The "surface height" is the fundamental BASIS for ALL depths in CAM, regardless of one's 'impressions' about what it might mean.

The surface of the stock is always ZERO (except in very rare instances).  Anything ABOVE the surface is a positive number, and anything BELOW the surface is negative.

It doesn't really matter "what works for you"... it's what's right. 

(sorry... this turned out to be a lecture, and all I was intending was to let you know how the system works... duh...  Still... It might be of value to someone -- I hope!)

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Dragonfly
CNC Jedi
*****
Offline Offline

Posts: 1929



View Profile
« Reply #6 on: May 25, 2016, 11:07:24 am »

I have observed such behavior - slow move at plunge speed instead of a rapid one to start point - many times. Sometimes it happens, sometimes not which perhaps means it depends on shape, size, tool and cutting parameters.
Never tried to find the cause. As in my humble opinion pocketing in CB has some, if not bugs then setbacks, and needs more attention for the next version. 
For this reason I often use a profile MOP with cut width > tool diameter instead of pocket MOP. Much more predictable behavior.
Logged

Before asking a question do some effort and walk through all menus and options in CamBam.  Maybe the answer is there. Please.
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1122


View Profile
« Reply #7 on: May 25, 2016, 11:33:09 am »

Unknown,
Not specific to your problem. The 0.6" hole with a 5/16" endmill would be better done with a spiral drill MOP as it would be faster and easier on the tool. That MOP does a great job and I often use it twice for larger holes, clear out the center then a second pass to size it.

I believe I have also seen the slow return to starting point issue, but I don't pocket very often.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5040



View Profile WWW
« Reply #8 on: May 25, 2016, 16:05:54 pm »

Hello,

Yes it sound like a bug ; the rapid move only appears if the tool diameter is <= to 0.23 for this circle diameter of 0.6.

with a tool = 0.3125, the rapids appears only for a circle diameter = 0.82 or bigger.

changing the step over or the max crossover distance has no effect. the rapid disappears if the tool is bigger that ~ 0.38x the circle diameter (the same pb appears in mm)

I'll add this to the bug list. Wink

++
David


* Sans titre-2.jpg (43.82 KB, 868x343 - viewed 131 times.)
Logged
Unknownpro
CNC Ewok
*
Offline Offline

Posts: 4


View Profile
« Reply #9 on: May 26, 2016, 03:36:14 am »

Let me first start by saying.... Thanks to all involved.

I was getting the job done at 35m17s with my original pattern. This afternoon I made a few design changes.

After I input the correct numbers depth (using a negative value) and changed the leadin to a spiral with a 15 angle I experienced less chatter on the plunge, no loss of speed on the return from completing a pass to the next and came up with a 27m13s design.

I still believe I can save more time, but I am still learning.

First time I have used the lead in/spiral with an angle, I need to do some more testing on what angles to use.

I am cutting aluminum for this project, and it's for a 80% lower if your wondering.
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3284


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #10 on: May 26, 2016, 15:45:41 pm »

Depths are ALWAYS negative of zero... zero being the surface of the stock, and positive being ABOVE the stock, while negative is below it.

Knowing full well this may muddy the waters there are circumstances where the stock surface may be above zero.  In those cases the depth should be less than the stock surface. 

Example:  You are doing secondary machining on a part with a boss on a larger surface.  You know the relative desired finish height of the boss in regards to the primary surface, but you do not know its current relative height.  Instead you take off the primary surface, and select a clearance plane and imaginary stock surface known to be higher than the boss. 

While I agree in principal I disagree in detail.  The depth should be less than the stock height.  If the stock height is zero than the depth will be negative. 

Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7559



View Profile
« Reply #11 on: May 26, 2016, 16:12:18 pm »

Yeah, yeah, Bob!  Wink

But before we start throwing in 'nuance', we have to promote 'the basics' (or at least "industry conventions").   Cool

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Pages: [1]
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.21 | SMF © 2015, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.326 seconds with 19 queries.

Copyright © 2018 HexRay Ltd. | Sitemap