[aldepoalo]

There are so many CAD CAM systems to choose from, which does what, how they REALLY work and what you get for the money.

So for those that are interested in participating, here is the challenge.

Use the supplied STEP file, document the steps to machine this part from start to finish.



gif hosting

[SCzEngrgGroup]

Some of the common low-end CAMs (SheetCAM, CAMBAM, etc) don't read STEP files, only DXFs, or DWGs.

Regards,
Ray L.

[BobWarfield]

Some of the common low-end CAMs (SheetCAM, CAMBAM, etc) don't read STEP files, only DXFs, or DWGs.

Regards,
Ray L.

Heh, that's good comparative information right there. Maybe someone with a nice CAD program that has lots of import/export can convert the files.

Good on you, Al. This'll be a good thread.

Best,

BW

[Bubba]

I agree with Ray and Bob, there is nothing I see that requires "3d" in that piece. My mentor who has YEARS of experience says that he has only used 3d machining a couple of times. 99%+ is 2.5D so why go to the expense of requiring it??
For that piece IF I had a dwg/dxf, I would do it in drafsight/sheetcam.

PS: I would also move the origin to a corner of the stock instead of some indeterminate point in the "middle"

[SCzEngrgGroup]

I agree with Ray and Bob, there is nothing I see that requires "3d" in that piece. My mentor who has YEARS of experience says that he has only used 3d machining a couple of times. 99%+ is 2.5D so why go to the expense of requiring it??
For that piece IF I had a dwg/dxf, I would do it in drafsight/sheetcam.

PS: I would also move the origin to a corner of the stock instead of some indeterminate point in the "middle"

Having 3D capability gives you a lot more flexibility in how you machine 2.5D objects. For example, you can use HSM techniques, instead of normal 2.5D roughing. It can make the job go faster. I'd love to have 3D capability for doing many of my 2.5D parts.

Regards,
Ray L.

[txcncman]

Deleted due to this being a thread to promote BobCad and not compare software.

[aldepoalo]

The first part of the challenge would be showing the steps for setting up the stock & work offset.

In BobCAD CAM V25 we use a stock wizard to automate this process. For those who don't know in the past when using BobCAD CAM software you needed to move your part to the zero. This is no longer the case!



1) File Open> Choose files of type, pick step and choose our sample file.


adult upload image

Now that the file is open let's setup the stock and work offset.


2) LT click on the CAM Tree Manager, RT click on Milling Stock, LT click on Stock wizard


image upload

From here we can choose our stock type, in this example we are going to use rectangular stock

3) LT click on arrows to advance the wizard.


gif hosting


By default the bounding box option is checked, if we want to add stock in X Y or Z you do so with the offset dialog

4) LT click Arrows to advance wizard

At this point we want to choose our origin ( work offset)



gif hosting



LT click on origin and then LT click on where you want your zero to be.

5) Once done LT click ok



image hosting adult


These are the basic steps for getting a part ready to machine.

Here is a video link walking through the same steps.

Setting up Stock - adepoalo's library

[Bob La Londe]

Some of the common low-end CAMs (SheetCAM, CAMBAM, etc) don't read STEP files, only DXFs, or DWGs.

Regards,
Ray L.

I haven't tried a STEP file, but CamBam certainly will handle STL or 3DS files. My CAD software can import and export all of those and more. I do 3D work with CamBam all the time.

I probably would not use 3D though for that part. I'll have to look again after I finish this post. Heck, I might not even import anything if I was designing and cutting that part. The 2D cad built into CamBam would probably be adequate to draw it too.

Ok. I admit it. When it comes to CB I can see that I am turning into a bit of a fanboy. LOL.

[BobWarfield]

For those who may need alternate file formats, I am uploading some. I was able to load Al's STP model into latest Rhino3D without incident. It did come up in metric and seems clearly to be an Imperial part (round numbers of inches, not so round numbers of mm), so I converted that for the alternate files.

Here is DXF and DWG attached. I also have 3DM and STL, but the uploader couldn't allow me to attach them--not a file format it likes apparently.

Cheers,

BW

[BobWarfield]

Having 3D capability gives you a lot more flexibility in how you machine 2.5D objects. For example, you can use HSM techniques, instead of normal 2.5D roughing. It can make the job go faster. I'd love to have 3D capability for doing many of my 2.5D parts.

Regards,
Ray L.

Ray, while there are HSM toolpaths that work in 3D, most are just 2 1/2D and HSM really has very little to do with 3D. HSMExpress, for example, gives you full HSM toolpaths with constant engagement angles for 2 1/2D, but has no 3D functionality.

If you have 2 1/2D software and are comfortable with it, and your part is 2 1/2D, I don't see a case where I'd want to use 3D toolpaths on those parts.

Meshcam makes a nice case for the idea that if you use 3D for everything and make it simple enough, it results in a very easy to use low end CAM product. But again, if I had 2 1/2D and was comfortable with it, I wouldn't use 3D toolpaths for it. They're way slower.

I'll have to see which CAM programs I have on hand I want to apply to this part.

One of the other interesting things to do if we can get all the way through to post, and if we can agree on a common post (should be Mach3 or Fanuc I would think) is compare the quality of the g-code produced. So you have 2 challenges:

- How easy is it to make the part?
- How good is the g-code as measured by its brevity and speed of execution?

We can measure speed of execution on any simulator. For example, my G-Wizard Editor will tell you how long a program is going to take. Most all the g-code editors will.

Cheers,

BW

[aldepoalo]

Bob,

The advance rough we offer can be used for 2D or 3D machining. The High speed cutting allows you to cutter deeper and run faster. But with that being said, you need to understand how it works in order to really use it best.

If you are working with open pockets we would use the advance rough to handle that as well.

[aldepoalo]

BobCAD CAM uses a Data CAM Tree Manager to store all your machining operations.

You'll use the CAM Tree to manage your setups, and machining features.



1) RT click on the Milling Stock



free image hosting

This is where you can choose the type of cutting you want. Drilling, 2D or 3D tool paths.


upload images


2) LT click on Mill 2 Axis




This will start our machining wizard. You want to choose the "feature" type for the machining operation you want to perform. In this example we want to start with a facing cycle. LT click on facing then choose next to advance the Mill 2 axis Wizard


hosting images


3) The next thing we need to do is select what geometry we want to face. In this example we are going to use the out side surface edges of our part. LT click on select geometry


free image hosting


Now you'll want to RT click on the surface edge and choose constant Z. Once the path you want to face in highlighted read hit your space bar.


adult upload image

The select geometry window will return with a preview of the geometry to face.


image upload

Then choose next to advance the wizard


4) At this stage of the wizard we are setting the rapid plane and top of part cutting.



gif hosting

Rapid plane is the save z position above the part for the tool to reposition. This is a non cutting position.

Top of part is where the tool path will start cutting from. You'll notice you have a pick top of part box which allows you to select your top of part off your geometry directly. In this example we will leave the default settings.

Choose next to advance the wizard

5) Posting



free picture hosting

This is where you can change your work offset or output a rotation angle. In this example we will leave the default settings

Choose next to advance the wizard


6) Choosing a tool

We have a few options for calling tools up out of your crib or tool library. In this example we are going to un check system tool and manually type in the information for the cutter we want to use.



jpg upload


You also will set your feeds and speed which will be populated from the material define in the job tree or you can edit the values as needed.


hosting images
Choose next to advance the wizard


7) Patterns

This is where we define the cutting motion of the face cycle.



image hosting

You have options to control if the tool cuts in 1 or 2 directions, the direction of cut, starting corner % tool to step over and if you want to shift the fist cut any amount.




8) Parameters

This is where you set stock for finish, cutting depth and increment of cut.


gif hosting


9) Leads

This is where you set the lead in value for the tool to approach and exist the work piece at



image hosting adult



10 ) Links

This is where you can set how the tool path links from one pass to the next


image hosting adult

11) At this point we choose compute to process the tool path. The result will be tool path displayed on the part based on our settings.



gif hosting



Here is a video link walking through the steps http://screencast.com/t/aWCAtSHFQsUh

[robgrz]

Here's a quick overview on how you'd do this in MeshCAM:

CAD/CAM Challenge - GRZ Software Blog

Being a 3D CAM program, it's a very different workflow.

-Robert

[aldepoalo]

Here is the sample G-code for the face cycle. Posted with a generic fanuc code ( mach 3)

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=3AXVMILL.MCH)
(MTOOL T1 S1 D2.5 C0. A0. H3. HT1 HD1.5 HH.5 DIAM_OFFSET 1 = 1.25)
(SBOX X0. Y-4. Z-1.125 L6. W4. H1.125)
(END PREDATOR NC HEADER)

(PROGRAM NAME: CAD CAM CHALLENGE.NC)
(DATE: WED. 06/20/2012)
(TIME: 12:41PM)

G90 G80 G40 G20 G17

(FEATURE FACE)

(TOOL #1 2.5 ENDMILL ROUGH)
T1 M06
M00
S800 M03
G54 X7.5 Y0.125
G00 G43 H1 D1 Z0.1 M08
G01 Z0. F3.
X6. F6.
X0.
G17 G03 X-0.4375 Y-0.3125 I0. J-0.4375
X0. Y-0.75 I0.4375 J0.
G01 X6.
G02 X6.4375 Y-1.1875 I0. J-0.4375
X6. Y-1.625 I-0.4375 J0.
G01 X0.
G03 X-0.4375 Y-2.0625 I0. J-0.4375
X0. Y-2.5 I0.4375 J0.
G01 X6.
G02 X6.4375 Y-2.9375 I0. J-0.4375
X6. Y-3.375 I-0.4375 J0.
G01 X0.
X-1.5
G00 Z0.1

G53 Z0
G53 Y0
M05
M09
M30
%

[txcncman]

I did not realize this was a "Promote BobCad" thread or a "Teach How BodCad Works" thread. All of the screen shots mess it up. You need to re-title the thread for your real intentions.

[aldepoalo]

"Use the supplied STEP file, document the steps to machine this part from start to finish."

I am the OP and I am documenting the steps start to finish using BobCAD CAM V25. I think MeshCAM did a good job of showing the steps of using his software and I look forward to other vendors / users documenting their steps as well.

We all can learn from this thread about how each package works, what they do and what they don't do. That is the intention of this thread if it wasn't clear.

[BobWarfield]

Here's a quick overview on how you'd do this in MeshCAM:

CAD/CAM Challenge - GRZ Software Blog

Being a 3D CAM program, it's a very different workflow.

-Robert

Robert, so glad you joined in!

For those who just want the simplest possible introduction to CNC and the easiest possible CAM, I have found it is hard to beat MeshCAM. In the original thread that spawned this one, the OP was arguing to start with simple CAM and get productive before you move on the Hard-But-More-Complete-CAM. If you wanted to take that approach, MeshCAM is a wonderful starting point.

Best,

BW

[MichaelHenry]

For those who may need alternate file formats, I am uploading some. I was able to load Al's STP model into latest Rhino3D without incident. It did come up in metric and seems clearly to be an Imperial part (round numbers of inches, not so round numbers of mm), so I converted that for the alternate files.

Here is DXF and DWG attached. I also have 3DM and STL, but the uploader couldn't allow me to attach them--not a file format it likes apparently.

Cheers,

BW

And here are versions in Alibre and IGS formats:

BobCADCAM Challenge Part - Alibre & IGS.zip

SprutCAM imports IGS files so that one might be useful for those (like me) using that CAM program.

I don't have time to do all the screen captures and such to document the way Al is, but importing, placing stock, and setting the workpiece origin were very easy with SprutCAM.

SC defaults to filling the footprint of the part with stock from Zbottom to ZTop so nothing was needed for that step.

Selecting the origin was a matter of highlighting the entire part from the Model tab, clicking on the "Transform" icon, selecting the "Locate Zero" tab and the clicking on "Min" for the X and Y axes and "Max" for the Z axis.

The rest of the programming took me about 45 minutes to finish, with 3 waterlining ops, two spot drilling ops, two drilling ops, and one hole pocketing op and with simulations after programming each op to make sure I didn't screw up somewhere and periodic stops to check G-izard for speeds and feeds. I only use SprutCAM a few times a month so it probably took me longer than it would have for someone experienced or even me if I was on a roll and doing several a day. I let SprutCAM pick default values for most of the parameters.

SprutCAM estimates that the job would take 6 minutes with HSS tooling and using G-Wizard suggestions for speeds and feeds. Based on past experience with similar jobs, I'd guess that the real job would take 7-8 minutes with a tool changer and 8-10 minutes with manual tool changes using TTS tooling that has been pre-set for length.

Mike

[neilw20]

I did not realize this was a "Promote BobCad" thread or a "Teach How BodCad Works" thread. All of the screen shots mess it up. You need to re-title the thread for your real intentions.

I AGGREE!!
And the screen shots are some CR4P link.
Do you want to report this stuffed up thread, or will I.

Has about the same appeal as the phone calls I got sick of.

[Gerry Sweetland]

I made a video and uploaded it to YouTube showing how I would set this part up using SprutCam.
I didn't bother with speeds and feeds but using G-Wizard I would of probably added another 5 minutes?
I also assumed the stock would be 1.25" thick.
I'm very new to machining so some of my choices may be fundamentally wrong but I'm learning as I go.
First time I have ever made a screen cap video with audio, sorry for the heavy breathing, I got a cold and thanks for watching
[ame=http://www.youtube.com/watch?v=85uZi4y9J9Y&feature=youtube_gdata]SprutCam part setup for machining - YouTube[/ame]
Gerry

PS
choose 1080p if you can, you can see the text on the screen better I think