Author Topic: Rest machining - for me, the "only" missing feature in CamBam!  (Read 12172 times)

Offline sibianul

  • Wookie
  • ****
  • Posts: 276
    • View Profile
Rest machining - for me, the "only" missing feature in CamBam!
« on: September 26, 2017, 06:58:10 am »
Hello everyone,

I don't remember if I talked to you guys about this feature, but now after a few months playing with Fusion 360 (I'm milling some steel small leather cutting dies) I think the Rest Machining feature is the most important one , that I really miss in CamBam. This feature it really saves a lot of time, time spent for doing CAM but also on actual machining time.

I would really pay easily $50 (or more) for an upgrade that would contain that feature, I'm really curious how many of you guys that payed for a licence years ago are willing to pay $50 or more for an important upgrade. I don't want to say that version 1 of cambam doesn't have many new features, I have both installed but still using the 9.8p version daily, I tried the v1 when a plugin didn't worked in the 0.98 version, I think dash lines plugin...

If the effort is really considerable, to implement REST MACHINING don't you guys think this would be the best way, for both parties: the developer / the consumer ?

Everyone, reading this topic, please reply  +1 if you are willing to pay (again) for this feature. I'm not the developer, but if I was, I would consider this option as the revenue will be much higher than just "waiting" for the daily sells to support the new updates.

PS. There is no poll option (anymore) on the forums?

Offline Dragonfly

  • CNC Jedi
  • *****
  • Posts: 2371
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #1 on: September 26, 2017, 07:35:47 am »
1. What is 'rest machining'? I didn't find a complete definition of it. As I understand it is a method using a tool with small diameter for finishing of uncut areas bu the larger tool.
2. Why is it impossible for you to use different tools in CamBam?

-1

Offline sibianul

  • Wookie
  • ****
  • Posts: 276
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #2 on: September 26, 2017, 08:23:35 am »
1. What is 'rest machining'? I didn't find a complete definition of it. As I understand it is a method using a tool with small diameter for finishing of uncut areas bu the larger tool.



Rest machining is meant to automatically compute the areas that remained unmilled from previous operation, and with current operation to mill only those areas. For example see the file bellow, I have an interior profile with a 3mm end mill, but because the corners overcut with this endmill with create a gap too large, I need to use a smaller endmill, in this case I will use a 1.5mm end mill, but because there is no REST MACHINING option, I have 2 options - feel free to give me some more advices :)

1. Option one is to use the small endmill on the entire profile, it will cut alot of air as it will actually mill only in the corners.

2. The second option is to draw another polyline only in the corners, and mill only those small polylines instead of the entire contour.

If the rest machining option was available, I will only use a profile operation with the smaller endmill, and the toolpath will be generated only in the corners where there remained some material unmilled material after the 3mm end mill.


2. Why is it impossible for you to use different tools in CamBam?

-1

It's not impossible, it's all about time lost by either altering the drawings, to only mill the small areas that remained unmilled, sometimes this is quite hard and time consuming, or by losing time while milling air at slow feed. If I use the same polylines with a smaller end mill, and the toolpath will be generated for the entire lenght, because of a much slower feed of the micro end mills (1mm or lower) there will be a huge time lost while machining, because it will mill air in 95% of the milling time.


UPDATE. I added another screenshot from Fusion 360 (I'm not saying CamBam is a very bad program, I love it, I said much often worse things about Fusion on their forum as it lacks some very basic features, also about rest machining, it has this option on contour operations and pockets, and 3D adaptive profile, but it does not has it yet for 2D adaptive profile, the operation I use it most for rough clearing )
So in the screenshot bellow you can see I chosed a 2D profile operation, and also selected the same geometry, the interior of the star, but the toolpaths is generated only in the corners. Belive me, this is a huge timesaving !!! That operation is done with a 1.5mm end mill also, but with a very very small DOC, just 0.08mm ... as I'm milling hard tool steel.
« Last Edit: September 26, 2017, 08:41:37 am by sibianul »

Offline pixelmaker

  • CNC Jedi
  • *****
  • Posts: 1778
    • View Profile
    • pixelmaker
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #3 on: September 26, 2017, 09:48:37 am »
Look at the script "unmachined areas" and the plugin "collision detector".

ralf

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3978
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #4 on: September 26, 2017, 14:40:59 pm »
Rest machining is a huge deal in finishing parts.  Not having it does cost me a lot of time.  I'll look at the unmachined areas plugin again, but I don't recall that it filled the need last time I looked it over.  I've asked for "rest" machining atleast a couple times myself. 

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

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3978
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #5 on: September 26, 2017, 14:44:48 pm »
I would pay an upgrade for significant improvements in 3D HSM (and 2D) and the addition of a good "rest" feature.  I can do those things in Fusion, but I am so familiar with CamBam that I struggle with the different work flow in Fusion360.  Also, Fusion is really 3D oriented.  It works best if you create 3D models of everything.  I've gotten used to working with 3D only for the organic portions of a job. 



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

Offline sibianul

  • Wookie
  • ****
  • Posts: 276
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #6 on: September 26, 2017, 14:58:19 pm »
Thank you Ralf, this script it seems to do half the job already (finding the unmilled areas)! so it's that simple to actually do REST MACHINING ... at least on simple 2D profiles ?

I don't know how others don't need / know about rest machining, for me it's a thing that I need daily, and because I don't have it I need to improvise, either by drawing the lines myself (now I won't do this again, the plugin Ralf told me about, does this just fine :) ) or by letting the router to mill air, like I did today, as I didn't had time to draw, and in the mean time, since the router was milling I was doing the CAM for another program.

PS. I don't do 3D profiles very often just 2D profiles and pockets, but almost every part has a pocket, that needs to have the corners overcut, main end mills for pocketing are 10 and 12mm .. but for overcut I use a 3mm end mill.
« Last Edit: September 26, 2017, 17:48:25 pm by sibianul »

Offline Dragonfly

  • CNC Jedi
  • *****
  • Posts: 2371
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #7 on: September 26, 2017, 15:57:06 pm »
I am doing such cuts and I suppose others also do. But I didn't know it's called "rest machining" :)
And I try to do it with what I have at my disposal. Anyway, I think for the purpose of fine finish the shape should be profiled with a finishing pass with the finer tool. So I always leave some roughing amount for the finishing pass. Pocketing the material at the places it's left uncut  is a bonus and a time saver. And it depends on the overall machined area. Sometimes one just has to be patient :)
I think a plugin, if not for complete MOP but which automatically makes the unmachined areas to shapes, is possible.
Here is a crude example. And in this case I used the 'Inlay toolpath' plugin to produce a shape suitable for a 4 mm end mill. Then applied 'Subtract' (new shape subtracted from the original) and got a few closed shapes at the corners.
« Last Edit: September 26, 2017, 16:01:10 pm by Dragonfly »

Offline sibianul

  • Wookie
  • ****
  • Posts: 276
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #8 on: September 27, 2017, 12:10:34 pm »
... purpose of fine finish the shape should be profiled with a finishing pass with the finer tool.

This is my problem, the finer tool are quite small, and the feed is very low, also DOC, so I either draw manually the unmilled areas (until now, from now on I will try to use the python script to automatically draw the unmilled areas) or I leave the machine cutting air while machining the entire profile, with a small tool, and low feed / DOC.

An option to do REST MACHINING automatically will be a time saver for anyone in my opinion !

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3978
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #9 on: September 27, 2017, 14:04:10 pm »
Sibianul,

He is talking about doing an entire surface with a finish pass.  That's good for a uniform finish, but it does not really address the fact that a shallow surface pass can be done an order of magnitude faster than the heavier cut areas where the larger cutter used for gross roughing was not able to go.  If you do the finish at the same rate as the clearing areas you turn hours into days.  LITERALLY.  If you do it at the shallow surface finish speed you break cutters. 

Do not over simplify rest machining.  Its important.  It will save time, money, materials, cutters, and improve over all part quality. 

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

Offline jk

  • Wookie
  • ****
  • Posts: 265
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #10 on: September 28, 2017, 11:32:19 am »
Read this topic and thought the collision detector plugin may be enhanced for a better workflow.

Right click on existing coarse MOP and select 'rest areas'. Plugin will lookup the tool diameter and clearance of
MOP. Then it would calculate the unmilled regions and put them to active drawing layer as shapes.

Then user could create new fine MOP manually with these shapes as source.

PS Maybe I'll write it if there is a request )
« Last Edit: September 28, 2017, 11:35:10 am by jk »

Offline sibianul

  • Wookie
  • ****
  • Posts: 276
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #11 on: September 28, 2017, 12:53:04 pm »
... doing an entire surface with a finish pass.  That's good for a uniform finish...

I also do a finish pass on all my exterior profiles (on parts that are thicker than 6mm, on those thinner, there is no need), sometimes on the interior ones also, especially if the initial roughing cut was done using multiple DOCs, but generally I do this with the same cutter, or just a slight smaller cutter, and at a higher feed, as it cuts 0.3mm, this is what I usually leave for the finish pass.

But REST MACHINIG for me is needed especially for the tight spots where even the 3mm end mill will not fit, on the CNC router I mill daily using the 3mm and 6mm end mills, those are the most used end mills, the larger 10 and 12mm endmill are used for quick pocketing, but there are also moments when I need to use very small endmills, and this is when REST machining will be a huge help for me. Also when milling brass leather emboss stamps, I work with very small endmills (3mm endmill is used for roughing, than 2mm one, than 1mm endmill for small areas, than start milling with 30 degree v-bits, first with a tip flat to 0.8mm, than with 0.1mm or 0.2mm tip size )  and vbits, again, the REST machining  option will be very very helpfull.

This CamBam software is quite amazing, I think every time I had an request you guys always "had another card to play", I wanted to easier do fillets -> you guys showed me the plugin for fillets and chamfers, when wanted V-engrave .. the plugin was already available, now asking for REST MACHINING .. you show me the plugin unmilled areas which is doing half the job :D I haven't tried collision detector yet.. but I'm prepared to be amazed again on what I can do with CamBam :) Love to work with it every day. As I also making daily progress in Fusion360 I found a few things that I still can't believe what a difficult workflow is needed to achieve simple tasks. Like centering one curvy shape/sketch insinde a rectangle, in cambam I need like 3 clicks and I'm done, in fusion I got replies from 2 different people with 6 minute workflow to be able to align at the center :))) Also measuring things seems more weird on some curved shapes, in cambam you click here and there .. and that's it, this is the size. In fusion you can't click anywhere you want ....

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4468
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #12 on: September 28, 2017, 13:39:49 pm »
I'm interested to know what happens with these 'rest shapes'.
Are they pocketed then inside profiled ? because if they are just pocketed then small parts are still left and if they are inside profiled then central areas are left.
As Dragonfly suggested, the inlay toolpath plugin can be used  and I have modified it do do just inside areas and I'm sure it would be fairly easy (famous last words  :D)  to do the full 'rest' operations if I knew exactly what needs done with them.
« Last Edit: September 28, 2017, 13:41:37 pm by EddyCurrent »
Made in England

Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3978
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #13 on: September 28, 2017, 14:39:37 pm »
Rest is a little more complicated than that.  If you are using for example a ball end cutter in an organic "pocket" you will leave a little ridge between the area cut by the first MOP and the second MOP using the method described using the uncut areas plugin.  Even with a square end mill in a flat regular pocket you will leave a little ridge on the sides.   Unless I missed something. 

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

Offline jk

  • Wookie
  • ****
  • Posts: 265
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #14 on: September 28, 2017, 14:45:53 pm »
I think these rest areas should overlap the coarse milled area a little.

See the attached picture and cb file as a general idea.

The logic is a little hard to follow, but anyway:
1) we got a green triangle to cut inside
2) offsetting triangle by coarse tool diameter will give us the internal edge we get after cut (yellow)
3) offsetting edge back by same diameter will give us external cut edge
4) subtracting this edge from original triangle leaves us with 3 uncut shapes (pale red)
5) now we want the coarse and fine areas to overlap, say, by coarse d/2. so we offsetting uncut shapes this much and get a cyan shapes.
6) now the intersection of these cyan shaped and original triangle gives us the areas for fine machining (magenta)

And they could be pocketed now.