Is CUT3D right for me?

This forum is for general discussion about Cut3D

Is CUT3D right for me?

Postby injunear » Sat Jun 02, 2018 8:18 am

Hi there.
A brief introduction. I've been using CUT2D for a few years on my CNC Router and am quite fluent cutting 2D parts. I now want to make parts on my Harbor Freight CNC mill. I have one part in mind (shown in the photo below) and want some information regarding whether or not this is the right application for my needs.

I should say that the fidelity to the part outline should be close and within reason. The shape of the part is not 90^ and there's a critical angle that needs to be maintained.

My first question would be:
1) Referring to the photo below, would this be a 2 sided part or a 4 sided part?
2) Assuming you have more experience than I with CUT3D, how would you orient the part in the body of the material to cut it efficiently?
3) How critical is the dimension of the stock it is to be cut from? If it's not perfectly square on all 4 sides will that cause error in the part after relocating and “flipping”?
Anything I should know that you know from your experience having cut some parts that I should know?

4) When I hear the term "flipping the part" how am I to do that? Taking the bottom edge of the part and rotating to the top? How about the two remaining sides (assuming 4 sided cutting)? I haven't found any videos that are clear in part orientation while cutting other than the initial setting.

Thanks much,
Bob T.
Image
Image
injunear
 
Posts: 4
Joined: Fri May 18, 2018 5:19 am
Model of CNC Machine: Seig (HF) CNC Mini Mill

Re: Is CUT3D right for me?

Postby LittleGreyMan » Sat Jun 02, 2018 9:29 am

Hi,

Difficult to answer as we require much more information:

-what is the size of the part?
-what material?
-is it a finished part? a foundry pattern? Can it be hold by screws, and can you fill them after machining?
-it's difficult to evaluate undercuts without a 3D model

machining precision is another story

This part may be doable with a 3 axis machine, bit you'd rather begin with something much more simple. This one requires mastering all the basics.

Depending on the material and the size, 3D printing may be a good solution. If it's a small part, you can probably forget FDM technology.
Best regards

Didier

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 858
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: Is CUT3D right for me?

Postby ger21 » Sat Jun 02, 2018 1:28 pm

I would not use Cut3D for that. It looks like the two ends are the only critical sizes parts ?
I'd rough cut the shape, and calmp it with each end sticking up, and use 2D toolpaths on each end.
Gerry
ger21
Vectric Wizard
 
Posts: 1222
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: Is CUT3D right for me?

Postby injunear » Sat Jun 02, 2018 9:00 pm

LittleGreyMan wrote:Hi,

Difficult to answer as we require much more information:

-what is the size of the part?
-what material?
-is it a finished part? a foundry pattern? Can it be hold by screws, and can you fill them after machining?
-it's difficult to evaluate undercuts without a 3D model

machining precision is another story

This part may be doable with a 3 axis machine, bit you'd rather begin with something much more simple. This one requires mastering all the basics.

Depending on the material and the size, 3D printing may be a good solution. If it's a small part, you can probably forget FDM technology.


The part will be made of Aluminum and cut from a 6061 block 3x3x3 or similar. The part dimensions are shown below.

I am NOT unfamiliar with CAD or CAM or machining parts. I currently cut many parts on my router and this Mill in CUT2D. I have nearly 5 years doing so. This part requires a minimum of 2.5 axis machining and I don't have 2.5 axis CAM. CUT2D CAM is very similar in look and feel to CUT3d from what I see. That's why I'm asking because I don't want to learn an entirely new CAM package.
Hence, my question is whether CUT3D will do this part with reasonable shaping results. If necessary I will machine the ends flat afterwards. I designed the part in other software and have a STL file.

I have fixturing plates that will hold the 6061 cube to the mill. I'm aware of the placing the part in the cube to allow the end mill to clear the fixture. I also use machinable wax to test paths before committing to cutting a part (depending on complexity).

My questions about the orientation (flipping) is simply to satisfy my own curiosity. I of course could learn empirically. It's not the important at this time.
I think I will orient the part in the material favoring the top of the cube with my part flat. What do you think?

Here's the photos I have of the actual part and some dimensions. The part uses a connecting rod on both ends to attach to other components. These are not part of this discussion as they will be installed (surfaces milled and holes drill after machining in CUT3d).....

Image

Image
injunear
 
Posts: 4
Joined: Fri May 18, 2018 5:19 am
Model of CNC Machine: Seig (HF) CNC Mini Mill

Re: Is CUT3D right for me?

Postby LittleGreyMan » Sat Jun 02, 2018 9:31 pm

Sorry, but it's difficult for me to explain how I'd machine this part in English and describe the different steps. I'd use mountings and hold the raw material with screws in the locations where you will drill holes.

Mastering 2D CAM is not the same than machining 3D parts. This is not 2.5D but 3D.
Best regards

Didier

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 858
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: Is CUT3D right for me?

Postby LittleGreyMan » Sat Jun 02, 2018 9:34 pm

I just see Gerry's answer. Yes, use 2D toolpaths at each end.
Best regards

Didier

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 858
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: Is CUT3D right for me?

Postby injunear » Sat Jun 02, 2018 10:30 pm

Well, frankly I don't think this is all that difficult. I'll post up a photo of the finished part.

Oh, the other software that I use is limited to 2.5 axis for the 'free version, unlicensed version'....I'm a retired engineer and don't have access to a licensed version anymore. I don't care to relearn CAM in the other package when after having downloaded the Trial for Vectric it's very similar to the CUT2D setups.....

Thanks for the help anyway.
injunear
 
Posts: 4
Joined: Fri May 18, 2018 5:19 am
Model of CNC Machine: Seig (HF) CNC Mini Mill

Re: Is CUT3D right for me?

Postby injunear » Thu Jul 26, 2018 5:51 am

So, after plopping down my cash to buy a licensed version of Cut3D I promised photos after making my first part. I cut my parts on my converted 3D Mini Mill using my very basic knowledge of Mach3 and other skills as noted below. Before that I want to assure anyone reading this posting that if you have 2D cutting and machine skills you indeed can do this.

Here's the skills you need to master:
>Mach3 (if that's what you're using for your machine). You need to master skills regarding pausing, stopping the quill and jogging off the part in the event of cutter breakage (or coffee break, whatever). Additionally, you need to know how to setup the work offsets so that you can get back to your workpiece point of reference and run the cut file from where you left off.
>You need to know how to fixture your part. In this case it's a no brainer, it's held by a vice.
> You need to know how to tram your table and the fixture.
> You need to know how to use an edge finder (used in conjunction with work offsets mentioned above)
> You need common sense....

Anyone that's been cutting 2D parts for a year or more likely has these basic skills.

There was indeed a learning curve I had to go through regarding 'feeds and speeds'. I finally settled on 2 ipm, 2500 RPM (you can't get anymore from a Mini Mill) and the depth of cut was set to 0.05 inch. The actual cutter speed for a 1/4 inch Ball Nose End Mill would be 4000 RPM. For an 1/8 inch ball nose End Mill would be 8000 RPM. Both are out of range of the Mini Mill. The 1/4 inch was used for roughing and the 1/8 inch for finish.

The stock needs to be square on all sides and flat on top and bottom. There's a few video online that address how to square a piece of aluminum.

After mounting the stock and setting the work offsets, you can start the process of rough cutting. Here's where you have to be very, very patient. My cut file went for 10+ hours/side....That's not a misprint....The Finish tool path takes another 4 to 8 hours depending on the option selected in CUT3D. There's a checkbox in CUT3D for the Finish to make a second pass perpendicular (at 90^) to the default Finish pass. In my opinion this is a waste of time. I see no tangible difference that matters and you can easily remove the material using an abrasive pad in a grinder made for such purposes (3M Scotch-Brite LD-WL Convolute Silicon Carbide Medium Deburring Wheel - Fine Grade).

The part shown in the photos requires a few more 2D machining operations and so it will not be removed from the block until tose operations are completed. It makes the part easy to fixture.

Image
Image
injunear
 
Posts: 4
Joined: Fri May 18, 2018 5:19 am
Model of CNC Machine: Seig (HF) CNC Mini Mill


Return to Cut3D - General

Who is online

Users browsing this forum: No registered users and 3 guests