CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
September 23, 2019, 10:24:25 am


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: I would like to try milling relief files in CB  (Read 2374 times)
huntleybill
Storm Trooper
***
Offline Offline

Posts: 146


View Profile
« on: June 12, 2019, 01:53:14 am »

I am somewhat confused on what I need to do to mill relief files. Instead of creating files, I thought I would download the files and use them. One file I downloaded was in stl format. When I loaded it into CB I could not setup tool paths etc. (of course). I tried exploding the file but all CB would do is think...and think,,,and think. Too much to process!

My first question is what format would be best for CB to process relief files. Stl does not seem to be working well.
Also, are there tutorials that step you through how to configure reliefs?

Thank you
Bill
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5554



View Profile WWW
« Reply #1 on: June 12, 2019, 02:08:11 am »

Hello

STL file is the right format (and don't explode it) ; you must use it with "3D profile" machining operations ; this is the only one MOP that can be used with mesh objects.

http://www.cambam.info/doc/dw/1.0.0/cam/3d.html

++
David
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5554



View Profile WWW
« Reply #2 on: June 12, 2019, 02:22:48 am »


this video show a 3D mesh made in CB (but you can import an STL too) and the use of the 3D profile MOP
https://www.youtube.com/watch?v=OLaX1Sa559w


++
David
Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 4007



View Profile
« Reply #3 on: June 12, 2019, 12:32:17 pm »

Bill,

I thought we had covered this subject, such as here; http://www.cambam.co.uk/forum/index.php?topic=6712.msg54315#msg54315
Logged

Made in England
huntleybill
Storm Trooper
***
Offline Offline

Posts: 146


View Profile
« Reply #4 on: June 13, 2019, 00:54:29 am »

Bill,

I thought we had covered this subject, such as here; http://www.cambam.co.uk/forum/index.php?topic=6712.msg54315#msg54315

Well. that is a little different. I got tired/frustrated with trying to learn how to make 3d reliefs from pictures. With this question, I want to learn how to import someone else's already created 3d relief and mill that. I was having issues getting it to work. Seems I was using the wrong MOP.

Also seems I forgot what I learned a year ago. It's a bitch getting old! Now, why am I here again?

Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 4007



View Profile
« Reply #5 on: June 13, 2019, 09:35:32 am »

Bill,

It's the same process, just import the stl, which as far as CamBam is concerned is a 'surface' just the same as ones you created of the dog etc.
Then add one or more 3D MOP in the same way you did for the dog etc.

Attach a cb file if you want further assistance, you might have to zip it if the the stl is big or choose a smaller stl file.
Logged

Made in England
huntleybill
Storm Trooper
***
Offline Offline

Posts: 146


View Profile
« Reply #6 on: June 17, 2019, 20:27:39 pm »

Sorry it took so long to get back to you on this. Life rudely interrupted my CNC play time!

I can't upload the file because it is too big. Even zipped. So, I have attached a picture of the stl file I was attempting to mill. (capture.png)  I uploaded the file into CB using the instructions Eddy previously gave me. I made changes to some settings for this milling job but basically followed the instructions.

The second picture (thumbnail) is the result. Almost no detail. I tried this file using different bits, different size files etc with no better results.

So, I went back online and downloaded the height map file (rose), read through the instructions on milling height maps with CB and I have attached the CB file setup as per the instructions.

I don't understand why CB automatically sets up the MOP as an engraving tho. I set it up to mill on a piece of foam, and I am glad I did. It took my 1.6mm bit and plunged it 10 mm into the foam, then started milling. If this was wood, it would have snapped the bit.

I had left the settings "depth Increments" at the default 0.4 and the target depth at -0.4. But it plunged at least 10mm into the stock! Because the test stock is foam, I let it continue to mill but is there a way to have the machine mill from 0 to the target depth instead?

It looks like it is milling correctly so I am thinking I would get much better results with height maps for milling reliefs like these, right?? But then I gotta learn how to make height maps!! Does this ever end?


* Capture.PNG (383.08 KB, 519x565 - viewed 40 times.)

* thumbnail.jpg (96.84 KB, 810x1080 - viewed 40 times.)

* rose.jpg (8.47 KB, 224x225 - viewed 32 times.)
Logged
huntleybill
Storm Trooper
***
Offline Offline

Posts: 146


View Profile
« Reply #7 on: June 17, 2019, 20:29:02 pm »

I couldn't squeeze the CB file in on the last post, so here it is.

* Rose.cb (5539.58 KB - downloaded 18 times.)
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5554



View Profile WWW
« Reply #8 on: June 17, 2019, 21:56:24 pm »

Hello

Quote
I don't understand why CB automatically sets up the MOP as an engraving tho

It's the normal way with "heightmap" ; it use engraving MOP.

You must use a target depth = 0 with the engrave mop, because the TD is relative to the polyline, not an absolute Z position as for other MOP.

If the tool down to -10, it's because your polylines goes to -10 ; if you want a smaller depth, you must set it in the Heighmap window, when you convert the picture to toolpath.

Heightmap is an "old" feature ; prefer the Draw/surface/from bitmap, that use regular 3D profile MOP and is better if you want to machine with more that one depth pass. (see attachment)

http://www.cambam.info/doc/dw/1.0.0/cad/draw-surface.html

++
David

* Rose_bitmap2surface.zip (791.8 KB - downloaded 43 times.)
« Last Edit: June 17, 2019, 22:09:24 pm by dh42 » Logged
huntleybill
Storm Trooper
***
Offline Offline

Posts: 146


View Profile
« Reply #9 on: June 17, 2019, 22:11:52 pm »

Thanks David, but draw/surface/from bitmap IS what I was using. The picture I attached previously showed the results.

The machine just finished the height map of the rose. I have attached a picture. As you can see it is MUCH better than draw/surface/from bitmap.

So, if there is a way to have the bit mill from 0 down to -10 in steps, I think it would work. OR, if there is a way to mill starting from a corner and mill on a 45 degree angle instead of horizontal or vertical, it would drastically reduce the stress on the bit.

No? Yes?


* thumbnail (1).jpg (77.96 KB, 1080x810 - viewed 42 times.)
Logged
huntleybill
Storm Trooper
***
Offline Offline

Posts: 146


View Profile
« Reply #10 on: June 17, 2019, 22:17:15 pm »

If the tool down to -10, it's because your polylines goes to -10 ; if you want a smaller depth, you must set it in the Heighmap window, when you convert the picture to toolpath.

The depth of the object is not a problem. -10 is ok with me. It's my tool that does not like to be plunged in 10mm then dragged across a piece of hard wood. If we can make it go down 2mm at a time until it gets to -10mm, I think the tool will be happier ..... and in one piece.  Grin
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5554



View Profile WWW
« Reply #11 on: June 17, 2019, 22:18:58 pm »

Quote
Thanks David, but draw/surface/from bitmap IS what I was using. The picture I attached previously showed the results.

Maybe for the bird, but for the rose.cb file you shared, it's not a surface but just a polyline made with Heightmap plugin.

Try to zip the .cb file of the bird ; if it is smaller that 4MB, it can be attached to the message.

++
David
Logged
huntleybill
Storm Trooper
***
Offline Offline

Posts: 146


View Profile
« Reply #12 on: June 17, 2019, 23:40:50 pm »

Hi David
I did try to zip it. Best I can get is 8MB. Says file is too big.

So ,Are there instructions for setting up the rose file? I did a draw/surface/from bitmap with it but do I follow the same directions Eddy gave previously?
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5554



View Profile WWW
« Reply #13 on: June 17, 2019, 23:51:01 pm »

have a look on reply 8 ; the rose done with "surface from bitmap" is attached Wink

I use X Width = 100
X grid step over = 1
min = -10
no changes for other values. (0 for all)

++
David

Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5554



View Profile WWW
« Reply #14 on: June 18, 2019, 00:18:18 am »

re

I discover something ... while playing with both surface2bitmap and heightmap on the same picture (the rose)

With the same settings for both methods, the result is ... that the polylines created by the heightmap method exactly follow the 3D surface created with surface2bitmap ..... nice, but ... the polylines are the "toolpath" used by the engrave mop, but the surface2bitmap generate compensated toolpath depending of the tool profile, so the resulting toolpath are not the same for the both methods  ...

maybe it's not a real problem, because in both cases, the source is an image ; not the better method to obtain a nice and accurate 3D model ... but it's interesting to know than the result is not the same with the 2 methods.

++
David
Logged
Pages: [1] 2
  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 0.15 seconds with 20 queries.

Copyright © 2018 HexRay Ltd. | Sitemap