[REVCAM_Bob]

Question: If I were to post a drawing of a simple die detail, or an autocad
drawing that could be downloaded, how many people would be willing to get
the drawing, and report back how long it takes to program the block for c.n.c. machining useing there CAM system. It would be an interesting measure of speed/ ease of use for CAM systems. If enough people respond
that they would be willing to do the sample programing, I will proceed. Maybe it could be set up as a poll?

[Cold Fusion]

I'm in with Onecnc.

[REVCAM_Bob]

What would be the best way to post the drawing? I have a pdf version of the
drawing and also an auto cad...perhaps the pdf version would be best and
attach as an image?

[lakeside]

I'm in with Bobcad 21 and Powerstation pro/plus(need a DXF or IGES for powerstation it can't open a DWG) If your part is a solid an iges would be a good format for a test.

[REVCAM_Bob]

How can I attach a file or files?

[Cold Fusion]

Zip the dxf file before attaching it.

[JFettig]

How about you PDF it and have people draw it in the cam program as well to show how long it takes to do both.


Jon

[rmtucker]

I,ll give it a go in alphacam/mastercam x/Catia

Mark

[REVCAM_Bob]

O.k. here is the stuff. In the zip file is a PDF print out of the dwg file, there is a dwg file, an iges file and a dxf file. It is all 2-d data.

The goal is to see how long it takes to do the programming on the block assuming it came from your "native" cad system. In other words, don't count converting this to the format you need to program as part of the programming time. For example, if you want to program it from a solid model, keep track of the time is takes to convert it to a solid model separately, but please tell us the conversion time also as it might be interesting to see.

Start with the assumption that the block is cold rolled steel bar stock saw cut to 5.12 inches long, the other dimensions are 2.000 x 4.000 as crs comes in pretty close to size.

To make sure everyone compares apples to apples the following should be programmed:

1. Square the block up on all 6 sides leaving 0.005 grind stock on each side. Do this with whatever machining practices you deem most efficient.

2. Machine 0.020" chamfer on all the edges of the block.

3. Do all of the drilling etc. including milling in the text 0.015 deep approx.

4. Program also from back side of the block to chamfer all the holes drill thru or to finish an features that could not be reached from the top side of the block.

5. Include in your time study a breakdown of how many different setups in the vise
(or however you would hold the block) are necessary to complete the block.

6. Happy programming.

7. If you have any questions that need to be asked, do not include them in your programming time..... My apologies if it is not all perfectly clear.....

Any other "Rules" you guys think should apply before getting started?

Thanks, Bob.

[REVCAM_Bob]

Second try at here is the zip file.................

[lakeside]

this is a simple type part to program here's you ingraving with x and y lower left also add pionts for hole location less than 5 min spent so far and now it time for long week end enjoy and rember the ones that are still on patroll

[ChrisJ]

Well I thought I would take a shot at this example.

So, using OneCNC Expert, I modeled the part. It took about 10 minutes. I didn’t rush plus I needed to look up the countersink diameter for the SHCS and tried to find some information on jack screws but came up empty. I’m not a machinist so I am not as familiar with some items as others are.
Then I programmed the toolpaths. This took about 15 minutes, maybe 20 at most. I am sure this is considered slow, but hey I am still learning. Maybe I can learn something here by others critiquing my methods, since my methods come from reading books and posts on forums and no practical experience. Here are my toolpaths:

1. Facing 1 – Top of stock programmed at Z0. Took off 0.015 in Z with one facing pass. Used a 2” face mill.

2. Facing 2 – Bottom of stock. Programmed bottom of stock (top of parallels at Z0), with one facing pass at Z1.97.

3. Facing 3 – Side of stock programmed at Z0. Took off 0.07 in Z with one facing pass. Used a 2” face mill.

4. Facing 4 – Opposite side of stock. Programmed bottom of stock (top of parallels at Z0), with one facing pass at Z3.86.

5. Facing 5 & 6 – Ends were programmed with a profile toolpath. Assumed that the stock is held in a 4” vise. Programmed with a 1” end mill, 0.1” depth of cut.

6. 3/8” SHCS – Programmed with a center drill, drilled thru and counterbored with a 0.5” end mill (helix style toolpath) for the countersink.

7. 3/16” holes – EDM – drilled thru.

8. 3/8” JS – Programmed with a center drill, drilled thru and counterbored with a 5/16” end mill (helix style toolpath) for the countersink.

9. Text – engraved with a Cut Chain – Constant Z toolpath using 0.015” tipped bit, 0.05” down.

The model was utilized to create boundarys for the facing toolpaths and paths for the profiling toolpath, by extracting those edges. The hole wizard found all the holes in the model, so I didn’t need to extract any edges to create those toolpaths.

As I finished typing this I realized I forgot the chamfer on all edges. So in another 15 minutes (only because I kept changing my mind and then realized some of my lead-ins/lead-outs were on the wrong side of the holes) I generated a chamfer toolpath for the top face for the edges and the holes. Then the bottom face plus the holes. Each was created with part set at Z0. Then the two ends had a chamfer toolpath on the two remaining edges on both ends. Part set at Z0 and the same toolpath ran twice for both ends.

I didn't program the chamfering of the holes from the back side, but from what I have read I guess this can be done with a dovetail tool and I am sure there is a toolpath in OneCNC that can be used for this, just haven't tried it.

Regards,
Chris

[REVCAM_Bob]

Good job ChrisJ I really like the solid model. Encourage some of these other guys
to take a crack at it also, maybe we can all learn some about how others do things...

[PoppaBear10]

Hey,

I did the part in OneCNC expert as well. I did it two ways one all in OneCNC and one in Rhino CAD, then transfered to OneCNC. Since Chris above had already did it in onecnc...I had a little head start on a good example of how to do it.

Note: I don't know what PLCS or Jack screws, or SHCS is, still dont, but I just was able to knock off about 10-15 minutes doing the CAD in Rhino just because I have used it much longer.

There are some things that I didnt understand on the part requirements. You didnt put the final size of the block. I know the stock is starting with 2x4 inches, and 5inches in length. I didnt understand what you meant buy leaving grind stock on the all the sides??? does that mean instead of 2" thick by 4" thick you would want it 1.990 x 3.990 x 5.005?? if so, then it took me about 20 minutes using Rhino for the CAD, and about 33 minutes in pure onecnc.

BTW: the two holes roughly in the middle the diameter was not given, I guess they are 3/16? What is a EDM start hole?

(sorry for the questions, but I am unfimaliar with the above listed abbreviations, I thought EDM was a solid electrode machining type???)

s

[Cncjunkie]

I'll do it in esprit tomarrow

[HuFlungDung]

Well Chris, you did well at under an hour.

I spent about 20 minutes making the model and various copies in 3 different machining positions, and another 70 minutes programming, rechecking the program and editing my process names to make the program understandable.

That's just me, and the way I work. I could have knocked 30 minutes off if I was less thorough, but the program would not make a lot of sense to me in a year, nor to the machine operator right now

Whoops, see already I forgot a few M0's near the beginning for each part flip. Oh well... back to the computer

[ChrisJ]

One thing I learned from this experience is that I think it would of been better if one of two things below were done a different way:

1. The dimensions on the drawing included the 0.005 leave for grinding on all sides. When machining the part it was very confusing to add 0.005 to the machining process and to the hole locations.

2. or I should have modeled the part with the 0.005 added to the appropriate dimensions so that performing the toolpaths is a slam dunk with out racking your brain and remembering to add (or substract) this value to the machining process or moving the model 0.005 off of X0 and Y0. For instance your jack screw which is shown with a counterbore which is 1.460 down is technically 1.465 down. The SHCS are not 0.4 down but 0.405 down. All the hole locations are +0.005 for the X0Y0 origin. I'm confused already just typing this.

Also to be fair, I modeled the part in one setting, came back the next day and performed the toolpaths. So, I did think a little (or maybe a lot) on my approach before I got started on the toolpaths. If I had spent the time figuring out the method without thinking first, heck it could of added an hour easy. Plus as Hu did in his attempt, I didn't add notes and such so that coming back to this a month or year later I would remember all my part locations and settings. I also didn't make multiple copies of the model. I only had one and left it at X0.005Y0.005Z-0.005. So, for two toolpaths that were above Z0, the Z01.97 and Z3.86 ones, I didn't have a pictorial representation during the simulation or toolpath preview. It certianly would help to remember all the processes better had I did this so that coming back to this months later it would make it easier to remember.

I hope I didn't insult anyone by posting short time cycles since I could have easily added 2X or 3X's that time in providing a well documented program which I did not do in this example.

Regards,
Chris

[HuFlungDung]

Chris,
I agree, that finishing allowance does throw a wrinkle into the works. One would wonder, what kind of chamfers do they expect to have after grinding? As well as that, the hole depths probably are not that critical that .005 is going to make or break the project. The tolerances on a real drawing might permit one to make this assumption without contacting the buyer.

For the facing operations, the method I would use would be to set the work offset so that the Z0 reference would be at the height of the common bottom reference of the part, plus the finish thickness of the part in that orientation.
So, if G54 Z = 1.960 + .010
G55 Z = 3.85 +.010
G56 Z = 5.0 +.010

Then, for the first facing of the 2" stock, I would set the top of job to the top of the stock at Z.03 and face down to Z .015 followed by flipping the part to the opposite side, and set the top of job at Z .015 and face down to Z0. This should eliminate the need to keep readjusting the work offsets, and at the same time, permit programming the hole depths from Z0.

[ChrisJ]

Hi Hu,

My method of programming in this example, the finish facing pass on the opposite side for finished thickness for that side was to use the bottom of the stock (say top of parallels) as the reference point. So instead of machining down from Z0, which I know is the preferred method of programming I ended up machining at the thickness height of Z3.87 and Z1.97. I just didn't see another way to machine down from Z0 given that the stock is not exactly 2.0" thick and 4.0" wide, because you need to establish some known Z reference height.

If I understand your method for facing you are establishing Z0 as top of stock. But if top of stock is actually rough size 2.0" stock then you can't use it as a reference point or for tool touch off. I know you have a fool proof method, so can you elaborate a little further?

Chris

[PoppaBear10]

hmmm,

reading the above I further think I missed the objective on the grinding stuff. could someone clue me in on, do we assume that the model is the 2x4x5? or 0.005 less than that, OR, start the machine stock at +0.005 over that??

Hu, thanks for showing how a pro does it, I never even thought to detail my program, I just did the part to make it and go...

The requirments didn't say you where limited to 3axis, so I did it on 5 to speed up the whole machining process....... does it say somewhere that you can only use 3?

would you mind telling me what all those abbreviations mean above?

s.