CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
September 26, 2017, 20:39:48 pm


Login with username, password and session length


Pages: [1]
  Print  
Author Topic: Friend trying out CB  (Read 2943 times)
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7086



View Profile
« on: January 20, 2017, 11:53:39 am »

I have a friend who's trying out CB right now.  He says, "CamBam or MeshCAM, whichever I can get to work on this project first, that's the one I go with."

So, I don't 'do' 3D work, and need to advise him.  He needs to import a 3D object from Solid Works, then somehow delineate the outside profile of the piece (which makes excursions in all three axes), and do a simple outside profile cut of the perimeter of the piece.  

As seen in the pic below, it ALREADY has the 'plane shape' with the bend. It's now a square sheet with the bend cast in.  All he needs is to cut out two identical pieces from this molded sheet of goods, without spending a lot of 'air time' -- in other words, actually following the contour, so as to not waste cutting time.  And then, drill the six holes, which are 'flat' to XY.

The piece can be oriented 'flat' to the XY plane during cutting.  It's only shown on a tilt in the drawing to help see its shape better.

Advice?
LLoyd


* part.jpg (79.52 KB, 622x555 - viewed 87 times.)
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
10bulls
Administrator
CNC Jedi
*****
Offline Offline

Posts: 2035


Coding Jedi


View Profile WWW
« Reply #1 on: January 20, 2017, 12:49:58 pm »

If you have a plan and offset 2D drawing you could...

1. extend some lines either side of the side view then use Draw - Surface - Extrude.
This in effect makes a surface that describes the sheet you will cut the part out of.

Rotate this surface 90 degrees around the X axis

2. Import the outline of the part and position it over the sheet.

Use Edit -> Offset to create a 2D toolpath around the shape to allow for the tool radius.

3. Select the 2D toolpath line and the surface then Use Edit -> Surface -> Project Lines to surface.

4. Select the new 3D polyline, then insert an engraving operation.

(see attached).

This doesn't allow for lead ins etc, but if you want to get flash, at step 2 you could generate a profile machining operation, use Toolpaths to geometry, then project these toolpath lines onto the surface

EDIT: I just replaced the attached file with a lower resolution 3D polyline. (2k vs 28k points)

* 3dtoolpath.cb (222.88 KB - downloaded 43 times.)
« Last Edit: January 20, 2017, 13:13:40 pm by 10bulls » Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3066



View Profile
« Reply #2 on: January 20, 2017, 13:19:32 pm »

Looking at this I'm thinking it would be great if the Engrave MOP could have a 'tool offset' parameter that defaults to half the cutter diameter if enabled, then it could act like a Profile MOP that follows X,Y,&Z

'Roughing Clearance' seems to do nothing in an Engrave MOP so maybe that would do as the offset parameter ?
« Last Edit: January 20, 2017, 14:08:18 pm by EddyCurrent » Logged
kvom
CNC Jedi
*****
Offline Offline

Posts: 1383


View Profile
« Reply #3 on: January 20, 2017, 13:37:15 pm »

Not knowing the dimensions is potentially an issue.  I would turn the sheet so that the bend is upward and than just cut the profile with a tool that is long enough to cut both the bend and the flat portion.  And I'd drill the holes first.
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7086



View Profile
« Reply #4 on: January 20, 2017, 15:07:13 pm »

Thanks, all.  I will convey this info to him.

Lloyd
Logged

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

Posts: 4


View Profile
« Reply #5 on: January 20, 2017, 16:03:40 pm »

Thanks, all.  I will convey this info to him.

Lloyd

Hi Lloyd,  no need to convey... I found this today after coming here to search for a solution.  Thanks!

The bit being used to cut this part out is a 1.47mm PCB trimming bit, which only has a cutting area of 10mm so it can not be used as a long cutter to trim the profile without getting the Z axis involved.

The starting blank is about 160mm square, with the thickness being 1.5mm.

I would think these kind of CAM programs would have a feature that allows you to define an outline in 3D space and then the tool path is routed along that outline using all three axis.  It would be very inefficient to have to do some kind of waterline scan thing to cut this in a series of flat  layers like you would when milling something from a block-- the bit can make the full cut in just one pass.  People do this all the time when trimming 2D parts out of flat stock, but doing that same thing on a plane that is not flat seems to be an illusive feature.  MeshCAM can't do it either.

Logged
Garyhlucas
CNC Jedi
*****
Online Online

Posts: 987


View Profile
« Reply #6 on: January 20, 2017, 18:05:39 pm »

I do this kind of thing in CamBam. Extract the top profile from the 3d model. Copy 3d part and rotate to get a side view on the xy plane. Get profile of this view. Break polyline to get a polyline of top or bottom surface. Extrude the surface and rotate it to the xy plane. Project top view polyline onto side view surface. The new polyline is the tool path you want for engrave. Tough to explain, easy to do!
Logged

Gary H. Lucas

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

Posts: 2902


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #7 on: January 20, 2017, 19:14:45 pm »

I do this kind of thing in CamBam. Extract the top profile from the 3d model. Copy 3d part and rotate to get a side view on the xy plane. Get profile of this view. Break polyline to get a polyline of top or bottom surface. Extrude the surface and rotate it to the xy plane. Project top view polyline onto side view surface. The new polyline is the tool path you want for engrave. Tough to explain, easy to do!

Yup.  If you have the profile shape you can create an offset using the profile shape that is half the radius of the tool, and then project the line to the surface and use an engrave MOP.  Then drill the holes.  I don't see this as easily doable in meshcam at all. 

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
Pyronaught
CNC Ewok
*
Offline Offline

Posts: 4


View Profile
« Reply #8 on: January 20, 2017, 19:49:57 pm »

The method being described here seems like it would only work for an extruded shape.  While the part I'm currently working has an extruded profile, most of the parts I have to make don't.  The image below is a more typical part that I have to trim, which has to be done in two steps since the entire part does not sit in a single plane (ideally a rotary A axis could be used, but I'm just going to manually flip it over to keep things simple in the beginning).

Having to recreate geometry using lines projected from 2D views just seems overly convoluted.  I would think this type of operation would be common enough that you could just load in a 3D model and select a series of edge lines to define the tool path, then the software creates the offset path based on the cutting bit diameter.  Maybe Fusion 360 has  this capability?  I'm not the one paying for the software so I don't care what it costs, I just have to find the right software to use for the job.


* complex.jpg (151.8 KB, 997x632 - viewed 87 times.)
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4628



View Profile WWW
« Reply #9 on: January 20, 2017, 23:05:51 pm »

Hello,

Quote
Looking at this I'm thinking it would be great if the Engrave MOP could have a 'tool offset' parameter that defaults to half the cutter diameter if enabled, then it could act like a Profile MOP that follows X,Y,&Z

+10, it would be very useful

Quote
He needs to import a 3D object from Solid Works

With SW its easy to extend the edge of the 3D from a given "toolradius" before exporting the 3D shape so you can use directly the edge detect in CB. (at least for this object)

a little video

https://www.screencast.com/t/6DfItGVyaB

++
David
Logged
Pyronaught
CNC Ewok
*
Offline Offline

Posts: 4


View Profile
« Reply #10 on: January 21, 2017, 00:14:07 am »

I've discovered the free 2.5D CAM plugin for SolidWorks called HSMXpress.  WOW!  It looks like they have a feature that works like I described called "Trace"

Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2902


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #11 on: January 21, 2017, 15:59:18 pm »

FYI:  Fusion 360 does a lot of what you want atleast partly because its both CAD and CAM.  It will import solid part files as well.  I currently use it to convert solidpart files to step files and stl files. 

I've found F360 to have a pretty steep learning curve, but it might not be so difficult for a Solidworks user. 

F360 is free to try and free to use for hobbyists, startups, and small businesses.  Their is a subscription fee for its continued commercial use by businesses over a certain size. 
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
Pyronaught
CNC Ewok
*
Offline Offline

Posts: 4


View Profile
« Reply #12 on: February 04, 2017, 07:25:38 am »

HSMxpress is actually the same CAM engine used in Fusion 360, since Autocad makes it.  Having it built right into SolidWorks is really nice though, since your CAM setup is built right into the same assembly as your part model and you can quickly make changes to either the part or fixturing and see the results right away without having to export into a third party program.  I'm surprised there are not more tutorial videos on it though, given that it is free.  I guess the cost of SolidWorks keeps it away from most hobbyists.  The user interface is pretty self explanatory though and if you are familiar with the concepts you can pick it up fast.

Here's the part being routed using gcode generated by HSMxpress and their Linux CNC post processor.  It's not the same exact part pictured above, but a similar one:

https://www.youtube.com/watch?v=7ZoMBAamPjE
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2902


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #13 on: February 12, 2017, 18:37:37 pm »

I'm surprised there are not more tutorial videos on it though, given that it is free.  I guess the cost of SolidWorks keeps it away from most hobbyists. 

And small businesses. 
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
lector
CNC Ewok
*
Offline Offline

Posts: 1


View Profile
« Reply #14 on: June 29, 2017, 09:29:10 am »

Why there aren't any tutorial videos for a long time?
Logged

I need some help with fixing slots on my PC. Somebody knows how to repair it?
Pages: [1]
  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 0.166 seconds with 18 queries.

Copyright © 2008 HexRay Ltd. | Sitemap