CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
November 13, 2018, 22:09:32 pm


Login with username, password and session length


Pages: [1]
  Print  
Author Topic: "spikes" on finishing profile  (Read 1332 times)
Mark81
Storm Trooper
***
Offline Offline

Posts: 110


View Profile
« on: January 06, 2018, 17:47:19 pm »

Hi guys, this is my first attempt to carving a 3D profile (from stl object).
Here the cb file (19 MB): https://drive.google.com/open?id=1HOmf2rxHJ7xIapzN5JhaMXIabjNKDuZ5

First question: the finishing profile shows some "spikes" to the bottom of the stock. Are they correct?

Then, I'm not sure I'm doing the whole stuff right. I need to carve only the front face of the object and it should be cutted out from the stock (I mean, without any frame).
Hence, I set the target depth of the roughing profile to the stock height (I still need to add the holding tabs as described in the manual). Then, using the Z-resize function I can increase or decrease the machining height of my object (i.e. the maximum will be when the centerline lies to the bottom of the stock and the highest position to the top.

Would you please help me to understand if I'm doing it correctly?
Logged
pixelmaker
CNC Jedi
*****
Offline Offline

Posts: 1651


View Profile WWW
« Reply #1 on: January 07, 2018, 12:43:55 pm »

In the attached file I make som changes.

I add tabs. If you need more you can copy/paste one and write the ID number into the mop-
I add a polyline for boundary (2)

I change the  milling method to scanline, vertical for roughing, horizontal for finishing. This is not a object for waterline strategies.
I add a distance for the boundary of 4mm, enough to cut the corners.
I change the highest z-position to -0.5, because the highest parts are not cut in the finishing when object is at z=0
I change the target depth to -12.5mm, enough for this object
I change the resolution and step over to 0.1
I change the tool to a ballnose.

I make a zip file from the cambam file because I can upload it.

For this size (20mb) the 3d object has a bad surface.


ralf

* rose_edit.cb.zip (3841.97 KB - downloaded 36 times.)
« Last Edit: January 07, 2018, 12:50:52 pm by pixelmaker » Logged
Mark81
Storm Trooper
***
Offline Offline

Posts: 110


View Profile
« Reply #2 on: January 07, 2018, 13:55:16 pm »

Thank you very much for the time spent for me!
I have just few other questions:

  • would you mind to provide a rule of thumb for selecting the right milling method? scanning/waterline
  • is there a difference between a ballnose and a bullnose bit?
  • how to estimate the right resolution/step over/tool diameter?
  • a little OT: I bought this stl on the Internet, but as you pointed out is not very good. Where I can find better stl files? Are there some good reference websites?
Logged
pixelmaker
CNC Jedi
*****
Offline Offline

Posts: 1651


View Profile WWW
« Reply #3 on: January 07, 2018, 16:55:43 pm »

Toolpaths are always parallel in one axis.

Waterline toolpaths are parallel in the Z-axis. However, no "ground" can be milled. If the edge to the ground does not match the multiple of the depth increment, the next higher level is milled as the edge.
These toolpaths are more suitable for constructional 3D models such as those from CAD. It is necessary to calculate that the toolpaths correspond to the edges.

Scanline toolpaths are parallel in X or Y direction. They are more suitable for naturalistic models such as this flower.
The distance from surface to toolpath is measured in predetermined steps (resolution). Sharp edges and details are therefore only hit if the resolution is high enough.

Ball nose means that the radius is half the diameter of the tool.
Bullnose may have smaller radii.
Cambam can only calculate ball-nose cutters

For 3D milling, the tool diameter must be smaller than the smallest required details.
In this 3D object the leaf veins are thinner than 1mm. You will not be milled cleanly with a 2mm milling cutter.
However, this 3D object is too coarsely resolved to cleanly mill such details.

This 3D object is not worth any money.
Here is a directory of pages where you can load 3D objects. However, they are more for 3D printing.
I do my own 3D objects myself, so I can't help much. It makes sense to learn how to make the objects. In this case it is often enough to know how to create a relief from a 3D object.

For example, I would create this rose in such a way that I can quickly mill it in 3D without any details. I would engrave the fine lines, according to lines that can be projected onto the 3D surface in Cambam.

ralf
Logged
pixelmaker
CNC Jedi
*****
Offline Offline

Posts: 1651


View Profile WWW
« Reply #4 on: January 07, 2018, 18:45:59 pm »

What I do for you…

I repair the object (more then 240 holes, multiple edges, etc)
I polish the object to get a better surface.
I reduce the faces with smooth surface to 36k faces   Grin

Now it has without compression a size of 3.7mb  Shocked

If I use a 3ds file format the size of the uncompressed object is only the half.

ralf

* rose_edit(repariert)_36k.stl.zip (2607.46 KB - downloaded 30 times.)
Logged
Mark81
Storm Trooper
***
Offline Offline

Posts: 110


View Profile
« Reply #5 on: January 07, 2018, 19:50:56 pm »

Wow thank you very much! Did you use CamBam to do this?
Anyway, the original stl was 3854 kB instead of 3583 kB of the new one. It's the cb file that grows in size. Mine was about 19.8 MB, yours (just import the stl in an empty project and save it) is 18.7 MB.

You said: "Cambam can only calculate ball-nose cutters", but (at least) in version 1.0 both ball and bull are available in the tool shape menu.

I'm going to order some tools because I have only end mills right now. Then I will show a picture of this work!
Logged
pixelmaker
CNC Jedi
*****
Offline Offline

Posts: 1651


View Profile WWW
« Reply #6 on: January 08, 2018, 11:52:44 am »

hello

Quote
Did you use CamBam to do this?

No. I use "netfabb Basic" for the repairing. Netfabb Basic is no longer available. But for windows the free trial version, even after 30 days, works again with reduced functionality and has also the repair tools.

Polishing and reducing the faces I do with ZBrush.
I'm sure with the free "Blender" it goes the same way. You can use a modifier for subdivide the faces, then you do the polishing, also with a modifier or with the sculpt tool. At last you reduce the mesh to a small size with smooth surface.

Quote
in version 1.0 both ball and bull are available in the tool shape menu
Cambam calculate ball- and bullnose cutters in the same way, in the middle at the tip and with radius=1/2 diameter. Cambam cannot calculate a cutter with a cutting radius smaller than 1/2 diameter. No matter what you call the cutter…
You need a radius cutter with radius 1/2 diameter.

ralf
Logged
Mark81
Storm Trooper
***
Offline Offline

Posts: 110


View Profile
« Reply #7 on: January 15, 2018, 16:36:11 pm »

Thanks to your support I successfully machined a prototype in MDF! Next round is with beech wood.
Roughing with end-mill 4 mm and finishing with ball-nose 1 mm, cutting depth 10 mm. Working parameters (as reference): 1500 mm/min and 1 mm increment for roughing and 800 mm/min single pass for finishing.

I have the last question about. I felt very lucky to not have broken the 1 mm bit.
Using a 10 mm stock you should use also a 10 mm cutter, but they are more difficult to find (and I guess more fragile).

Actually, you DO need that only if the finishing path is close enough to a sharp edge of the material. In this situation a shorter cutter will crash with the shank. In this design this didn't happen because the edges are lower enough and the shank is above them. Mine has a cutting length of 4 mm.

I don't want to rely on luck again Smiley
Might CamBam tell me the minimum vertical clearance for a given tool diameter (cutting/shank)?




* roughing.jpg (120.29 KB, 800x600 - viewed 49 times.)

* finishing.jpg (163.16 KB, 800x600 - viewed 56 times.)
« Last Edit: January 15, 2018, 16:55:35 pm by Mark81 » Logged
pixelmaker
CNC Jedi
*****
Offline Offline

Posts: 1651


View Profile WWW
« Reply #8 on: January 15, 2018, 17:18:53 pm »

hello
I have special 3D milling cutters for this kind of work. The cutting edge of a 1mm milling cutter is 3mm long. Afterwards, the cutter is 8mm thinner than the cutting edge for a further 8mm. Only then does it go to 3mm shaft thickness.
There are extra long versions, e. g. 3mm diameter with 30mm length.
These milling cutters are specially designed for finishing 3D work.

Ralf
Logged
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 0.137 seconds with 20 queries.

Copyright © 2018 HexRay Ltd. | Sitemap