CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
January 23, 2018, 19:36:31 pm


Login with username, password and session length


Pages: 1 ... 9 10 [11] 12 13 14
  Print  
Author Topic: Trochoidal Pocket & Profile MOPs plugin (HSM)  (Read 26381 times)
dah79
CNC Ewok
*
Offline Offline

Posts: 30


View Profile
« Reply #150 on: July 26, 2017, 23:29:13 pm »

Machining a pocket in 6061 AL .25"deep.  Using the Trochoidal pocket MOP, and if I change the spiral feedrate slower than cut feedrate, it follows the spiral feedrate for the whole toolpath.  I just want to slow down the initial spiral to depth cut plunge rate.

For a temporary fix, I just created a circle and used a standard pocket MOP down to -.25".  And then ran the trochoidal pocket MOP with a start point at the previous circle center.  While this works, I thought the troch MOP would handle the initial plunge....
Logged
jk
Storm Trooper
***
Offline Offline

Posts: 228


View Profile
« Reply #151 on: July 27, 2017, 00:34:20 am »

A few options:

1) Lead Move Type: Spiral, Spiral Angle: 0, Lead Move Feedrate: desired feedrate
this will follow the full spiral backward, gradually going into the depth. First rev will be hard on a cutter (slotting)
next revs will be easier since a lot of material is removed.

2) Same but Spiral Angle: 1..5 degrees.
This will use the only a part of spiral for plunging, faster time but more cutter load.

3) Lead Move Type: Tangent, Spiral Angle: 1..5 degree, Tangent Radius: ~ tool diameter / 4
This will do the helical drill you probably want. But please verify the result with the 'show cut widths' enabled, in some cases it may be placed wrong and interfere with the pocket walls )

Logged
dah79
CNC Ewok
*
Offline Offline

Posts: 30


View Profile
« Reply #152 on: July 27, 2017, 13:01:46 pm »

I will try suggestion #3 and see if it works for me.  Another thing I noticed is that it doesn't get completely into the corners.  Is this possibly a setting I am missing?  Sorry for all the questions, but I had kind of gotten away from CamBam, but using this MOP is the best way for me to mill aluminum.



* Troch MOP.png (132.78 KB, 1079x644 - viewed 95 times.)
Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3290



View Profile
« Reply #153 on: July 27, 2017, 13:10:44 pm »

Another thing I noticed is that it doesn't get completely into the corners.  Is this possibly a setting I am missing?  Sorry for all the questions, but I had kind of gotten away from CamBam, but using this MOP is the best way for me to mill aluminum.

It's generally best to finish with a profile cut to clean things up so that would remove any left overs at the edges.
Logged
dah79
CNC Ewok
*
Offline Offline

Posts: 30


View Profile
« Reply #154 on: July 27, 2017, 13:16:35 pm »

Quote
It's generally best to finish with a profile cut to clean things up so that would remove any left overs at the edges.

Which is what I was doing, just wondered why it didn't get closer as the bit will fit in that area. 
Thanks
Logged
Dragonfly
CNC Jedi
*****
Offline Offline

Posts: 1792



View Profile
« Reply #155 on: July 27, 2017, 13:20:14 pm »

As I see it, the plugin's power is in bulk material removal for roughing. Therefore some finishing should be added too.
Logged

Before asking a question do some effort and walk through all menus and options in CamBam.  Maybe the answer is there. Please.
dah79
CNC Ewok
*
Offline Offline

Posts: 30


View Profile
« Reply #156 on: July 27, 2017, 13:23:19 pm »

As I see it, the plugin's power is in bulk material removal for roughing. Therefore some finishing should be added too.

I agree.  The plugin works very well for what I want/need!!  Just trying to make sure that I am not missing something obvious.
Logged
jk
Storm Trooper
***
Offline Offline

Posts: 228


View Profile
« Reply #157 on: July 27, 2017, 13:50:03 pm »

I will try suggestion #3 and see if it works for me.  Another thing I noticed is that it doesn't get completely into the corners.  Is this possibly a setting I am missing? 


There must be a little extra space between the tool and narrow channel to consider it millable.
Otherwise the trocho slices will transform into the straight slotting (180 degrees tool engagement angle) and a possibly broken tool. This extra space is about the 5% of the tool diameter.

If the corner is wide enough but not milled completely, try changing the Minimum Stepover. Say, 0.8 instead of default 0.9.
Logged
dah79
CNC Ewok
*
Offline Offline

Posts: 30


View Profile
« Reply #158 on: July 27, 2017, 14:06:50 pm »

Thank you for all the help.

Quote
3) Lead Move Type: Tangent, Spiral Angle: 1..5 degree, Tangent Radius: ~ tool diameter / 4
This will do the helical drill you probably want. But please verify the result with the 'show cut widths' enabled, in some cases it may be placed wrong and interfere with the pocket walls )

This solution worked for me.
Logged
kvom
CNC Jedi
*****
Offline Offline

Posts: 1429


View Profile
« Reply #159 on: August 15, 2017, 12:40:13 pm »

Yesterday I used the profile for the first time, and because I wanted to mill away all the stock around it I made the cut width large enough to do so.  However, I found that in doing so I was cutting air a lot of the time.  In retrospect, I realized that had I created a rectangle around the stock, the pocket version would have done the same thing with very little air cuts.

Experimenting, it seems that a rectangle large than the stock by the tool diameter in both dimensions was needed.

Thought I'd share.
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3076


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #160 on: August 17, 2017, 16:07:44 pm »

Generally I got better results with the pocket version of this plugin.  Sometimes I create custom shapes with a starting tab outside the stock.  Other times I create custom pocket and island setups.  I've found to really get the most out of this you have to spend a little more time thinking about the actual machining. 
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
kvom
CNC Jedi
*****
Offline Offline

Posts: 1429


View Profile
« Reply #161 on: November 24, 2017, 21:39:13 pm »

I tried the profile version again on some Mic6 aluminum, 1/2" thick.  Went .4" deep with .2" DOC and 1/2" cut width and .05 roughing clearance.  I didn't used mixed cutting this time and was surprised to see how good the finish was. 

I think this is a good option when cutting a fairly deep slot in aluminum and there is plenty of room for chip clearing (I just have air blast, no coolant).  Of course it's a lot slower than a straight profile.



I've pretty much settled on using the pocket op on all my parts where a toolpath can be generated.
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3076


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #162 on: November 26, 2017, 18:01:12 pm »

I think this looks like a part that would be best made with thicker than desired stock.  Remove all the stock on top that is not the part.  Then flip the part into custom machined soft jaws to remove the extra thickness.  It may not be fastest for one part, but for more than one I assure you it will be much faster.  Probably face milled off the bulk of the bottom, then flycut to thickness for finish.  

With this approach you could also use smaller (X/Y) stock which would save as much (or more) material as you would waste when machining off the bottom.  Joe Pi also has a great video on this on YouTube. 
« Last Edit: November 26, 2017, 18:03:36 pm by Bob La Londe » 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
kvom
CNC Jedi
*****
Offline Offline

Posts: 1429


View Profile
« Reply #163 on: November 26, 2017, 22:59:41 pm »

No argument there, but part is one-off, and I didn't have any thicker stock.  This project is a mechanical sculpture where most parts are one-off and have few if any straight sides.  About 150 parts.  The prototype is made from plywood so everything is a flat outer profile.

A few of these parts have 1/4" through holes that can be used to screw down to a fixture plate.
Logged
jk
Storm Trooper
***
Offline Offline

Posts: 228


View Profile
« Reply #164 on: December 04, 2017, 19:26:04 pm »

Hi.

Occasionally some pocket shapes failing to produce a good Voronoi partitioning -
slicing is going fine and then just stop for no reason, often steering towards the wall.

I'm thinking about swapping the underlying Voronoi routine to the more robust one from the triangle.net project.

If you stumbled upon some really bad partial slicing, feel free to post cb files (or PM me).
I need examples of bad partitioning for testing new code.

Example of such slicing below:


* bad_voronoi.png (107.16 KB, 1032x802 - viewed 46 times.)
« Last Edit: December 04, 2017, 19:29:49 pm by jk » Logged
Pages: 1 ... 9 10 [11] 12 13 14
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.124 seconds with 18 queries.

Copyright © 2008 HexRay Ltd. | Sitemap