[MichaelHenry]

I've got a round part that was turned on a lathe and am trying to figure out how to use SprutCAM to generate a toolpath to mill two flats vertically on opposing sides of the part.

The best I've come up with is a 2D contouring operation which is attached as a zip of the STC file but it also side mills around the periphery of the part.

The jpeg shows the flats to which I'd like to limit the milling operation, but I can't figure out a way to do it.

Can anybody suggest a solution?

Thanks, Mike

[Geof]

.....The jpeg shows the flats to which I'd like to limit the milling operation, but I can't figure out a way to do it.

Can anybody suggest a solution?

Thanks, Mike

Yes!!!! Learn enough G code so you can write this type of trivial little routine by hand. It is pitiful that you need a computer program to do something so simple.

[MichaelHenry]

Geoff,

It would be even simpler to use a manual mill, but I'm trying to learn how to use SprutCAM here, not focus on the quickest solution.

Mike

[SIG]

Yes!!!! Learn enough G code so you can write this type of trivial little routine by hand. It is pitiful that you need a computer program to do something so simple.

Why would you take the time to post? And not offer anything productive.
Like I just did.

[S4 Monster]

Hi Mike, In V4, 2D Contouring is the way in which I would do this too......
To stop the cutter running around the whole of the shape you should use partial machining.
When you select a 2D curve for machining, you can also dynamically drag the tool to where you want to start / finish machining.
What you may not realise is that you can drag the 'golf flag' at the centre of the tool to where you want the end of the machining to be.
To then extend the toolpath so that it approaches and retracts away from the part, you can use a 'Tangent' Approach & Retraction (Toolpath tab).

The file that you had attached was just the G-code file, so I have produced a mock up of your part in a V4 project for you to have a look at (attached).

In SprutCAM 2007 we can machine this part very quickly using the new 'Job assignment' option. This allows you to select the faces that you require machining, even vertical ones...which was a problem with V4:

[MichaelHenry]

To stop the cutter running around the whole of the shape you should use partial machining.
When you select a 2D curve for machining, you can also dynamically drag the tool to where you want to start / finish machining.
What you may not realise is that you can drag the 'golf flag' at the centre of the tool to where you want the end of the machining to be.

Wow, that's what I was wanting to do but couldn't find a way to accomplish it. I'm not at my SprutCAM PC now and can't check, but is partial machining the same as dynamically dragging the tool? Do you know if that is covered anywhere in the manual? I just ran a search on "partial" in the PDF file but couldn't find the term in there. I have seen the dialog box where can enter tool start and stop locations, but wasn't aware that the feature was also implemented graphically.

The file that you had attached was just the G-code file...

Sorry about that - I thought it was the STC file, but must have zipped the TAP file by mistake. Late nights do that to me.

In SprutCAM 2007 we can machine this part very quickly using the new 'Job assignment' option. This allows you to select the faces that you require machining, even vertical ones...which was a problem with V4:

That sounds like a really good feature. I'll have to try out SprutCAM 2007 *very* soon.

Mike

[S4 Monster]

Hi Mike, sorry but I don't do manuals The term 'partial machining' is one of mine.
I've created a short video to show you how it's done.......a picture paints a thousand words and all that.......enjoy:

Dynamic start / finish

Dave

[MichaelHenry]

Thanks a million for that video - I modified the operations parameters as suggested and finished the parts tonight with no problems.

Mike

[Don Clement]

Hi Mike,

I make flats on round parts in my Tormach. The part is held vertically in an EagleRock 5C collet fixture. The collet fixture is centered so that X0 &Y0 coincide with the centerline axis of the collet. I don't use SprutCam, but manually wrote G-code to have endmill mill flats on the side of the part.

Don Clement
Running Springs, California

[MichaelHenry]

Hi Don,

I used an Enco 5C fixture, probably similar to the Eagle Rock you used.

The feature was simple enough that I could have used MDI with Mach to do the milling, but the primary objective was to learn how to use SprutCAM a bit better.

Today I'm milling soft jaws for my vise and the lessons learned with the flats are paying off a little larger dividend.

Mike

[Don Clement]

Hi Mike,

I just installed SprutCam 2007 and am trying to mill an 11.86” diameter curve in a circular part held in a 3” internal expanding 5C collet held in the same EagleRock 5C fixture on my Tormach. The mill is a ½” diameter solid carbide ball end mill. As shown in the following photo there is a problem on the flat area in the center of the part whereas the outer edges are quite smooth. I originally created the G-code using SprutCam 4 and a waterline. I am now redoing this program using SprutCam 2007 and waterline but am still figuring out the new “fixtures” in SprutCam2007 vs “restrictions” in SprutCam 4. I believe if I check scallop height instead of using a fixed distance in the milling strategy that the rough areas in the middle will smooth out. I need to figure out the way “fixture” restrictions works in SprutCam2007 though. Any help with how to use” Fixture” and “restrictions” in Sprut2007 would be appreciated.
http://i72.photobucket.com/albums/i1...inDiaCurve.jpg

Don Clement
Running Springs, California

[MichaelHenry]

Don,

Wish I could help but I just got SC 2007 installed myself and am still finishing up my current project in SC 4. Maybe Dave will pop in and educate both of us.

BTW, SC 2007 looks pretty appealing from a visual standpoint.

Mike

[Don Clement]

BTW, SC 2007 looks pretty appealing from a visual standpoint.

Mike

I agree, SC 2007 looks prety good.

-Don

[davereagan]

Is this all a joke? It took me a lot longer to read through these threads than it would take to write a 4 line program to mill those flats on my CNC mill. Am I missing something? Is this being milled on an Integrex type lathe?

[S4 Monster]

In SprutCAM V4 we had restrictions which were used to define area's which we wanted to machine, and also fixtures (clamps - vices etc.).
In SprutCAM 2007 we describe the area's that we wish to machine using 'Job assignment' and fixtures....well using 'Fixtures'.

Under job assignment we can select the faces (Add faces) of the part which we want to machine, or we can select closed curves (Job zone) to define them, or we can use a combination of both.
If you wish to restrict machining from an area, you would select the curves in the 'Fixtures' section (or sub-section). You simply extrude the curve using the Top level and Bottom level amounts.
This is better than simple restrictions in V4 because we can give the restriction a height / depth.
You can still use curves in the 'Fixtures' section to restrict the machining to an area, but you have to select the 'Through holes' option......you need to add stock to allow for tool radius.
Note: if you are using more than one curve in this way, they have to be added as a Group i.e. in their own folder.

Don, your part looks good. You could improve things by using the scallop function.
Because of the shallow nature of the faces that you are machining, I think that you would probably get a better result by using the 'Plane finish' operation, possibly using a scallop height too....
Waterline finish is best used on surfaces that are steep, typically between 45 & 90 degree's.

HTH.

Dave

[S4 Monster]

Is this all a joke? It took me a lot longer to read through these threads than it would take to write a 4 line program to mill those flats on my CNC mill. Am I missing something? Is this being milled on an Integrex type lathe?

errmm....I think that the thread has moved on a bit from milling flats. How long would it take to manually write the program to mill Don's curved part I wonder?
The original thread was started by a new SprutCAM user as a question about doing a simple part programmed using the SprutCAM software. We all have to start somewhere.....once these foundations are laid then they will be machining far more complex parts with ease.

Dave

[Don Clement]

How long would it take to manually write the program to mill Don's curved part I wonder?

Dave,
Thanks for the help with SprutCam 2007.

Actually I did write a manual program to make the curve shown and manually machined this curve on my Rockwell vertical mill. This was before I got the Tormach PCNC. The method takes a series of cuts with a piece-wise incremental approximation of a circle using the formula: depth of cut = sqrt(R^2-d^2) + s -R where R=radius of curve, s=saggitta of base curve, d= distance from centerline of base. I made an Excel spreadsheet program to produce the coordinates for manual milling. The same Excel spreadsheet could be used to manually create G-code for a CNC program.

BTW I created a fixture model of the area I did not want to machine in Solidworks and imported the IGES file to the "Fixture" area in SC2007. So far I like SC2007 much better than SC4 but still have a lot to learn about SprutCam2007 vast capabilities.

Don Clement
Running Springs, California

[MichaelHenry]

Is this all a joke? It took me a lot longer to read through these threads than it would take to write a 4 line program to mill those flats on my CNC mill. Am I missing something? Is this being milled on an Integrex type lathe?

As S4 Monster replied, I started the thread in an attempt to learn something. My apologies if that offended you.

Mike

[davereagan]

No offense at all. Maybe I am jealous. I have not taken the time to learn a CAM system and a simple job like this is probably the perfect way to begin safely. I remember when I got my first CNC and had no training other than a Bridgeport. I had to make myself use the CNC machine. It took me 2-3 hours to do a one hour Bridgeport job, but I was laying the groundwork to be able to do that 1 hour Bridgeport job in 15 minutes a year later. After knowing the control and the tooling, I felt like I was cheating compared to using a manual machine and just holding my prices steady. Then I made some machine payments and didn't feel like I was cheating any more.

Dave