Machining car end?


grangerroads@...
 

I work only in TT scale (yeah, it's alive, barely, but friends of the scale are attempting a revival), one of my CAD/CAM projects at the moment is a transition era refrigerator car. Perhaps someone here has CNC-cut Dreadnaught ends and might be willing to give me a tip or two about approaching such a cut?

Thanks much,

Brian Chapman
Cedar Rapids, Iowa



destorzek@...
 

Do you have 3D surfacing capabilities?

Dennis Storzek


grangerroads@...
 

Dennis,

I have Rhino 3D but do not have 3D CAM software. And, I haven't yet taken the time to learn much of Rhino. I create drawings in AutoCAD 2D, recreate them in Inventor 3D to check part fit and appearance, then proceed to CNC-cut parts and assemble them for resin casting.

So far, I've cut simple round, smooth contours by manually placing tool paths at incremental cut depths of .001". Doing this with an IDE would be tedious, I know. . . .

-Brian Chapman
Cedar Rapids, Iowa


destorzek@...
 




---In STMFC@..., <grangerroads@...> wrote :

Dennis,

I have Rhino 3D but do not have 3D CAM software. And, I haven't yet taken the time to learn much of Rhino. I create drawings in AutoCAD 2D, recreate them in Inventor 3D to check part fit and appearance, then proceed to CNC-cut parts and assemble them for resin casting.

==================
Rhino should certainly be able to handle the model generation... What are you using for CAM software, if I may ask?

Dennis Storzek


grangerroads@...
 

> Rhino should certainly be able to handle the model generation... What are you using for CAM software, if I may ask? <

Vector CAD/CAM. It has a 3D module, but at the time I bought the package I didn't buy that.

You know the old adage, if you can't say anything nice about anybody, don't say anything? . . .

-Brian C.
Cedar Rapids, Iowa


destorzek@...
 




---In STMFC@..., <grangerroads@...> wrote :

Vector CAD/CAM. It has a 3D module, but at the time I bought the package I didn't buy that.

================

So, all you have to work with is a 2-1/2D CAM package.

SIDE NOTE: 2-1/2D describes the ability to move 2 axes concurrently, but only move the third while the other two are stopped. You can cut a circle with 2-1/2D, driving the tool around the curved perimeter in the XY plane, then increment the Z down while the other two are stopped. To cut a hemisphere, you need full 3D; all axes moving simultaneously.

It should be possible to cut a Dreadnaught end with 2-1/2D software. A number of years ago we had a machine control that was only capable of 2-1/2D motion, but we could select which two axes were active together. To do this end, I would build the solid model and orient laying on the flat back, then section it crosswise (across the width of the car) in small increments, then toolpath the mill to cut each profile in the ZX plane, incrementing in the Y to begin the next profile. You will need to finish with a ball nose tool as small or smaller than the smallest radius in the part. A .015" ball nose end mill should do, as a quick look at some drawings shows 7/8" to be the smallest radius, which is just a tad less than .0075" in TT scale, which is the radius of a .015" diameter tool. A .012 or .014 diameter tool would be better, but .015 is much more available. To get a smooth finish you likely want to increment over only .001 at a time. It's a lot of cuts, but you'll get there eventually. From experience, the "cusp", the ridges between each toolpath, will likely show the most in the fillets where each "wale" and "dart" blends to the basic shape of the end, and some contour toolpaths that follow the fillets around in the XY plane may be needed to smooth them out.

That begs the question of where to get the information to program the 3D model. NONE of the drawings published in the normal places have enough information. Drawings in hobby magazines are worthless, and the Car Builder's Cyclopedias only have what are called General Arrangement drawings. The purpose of these drawings is to show how the parts fit together into the whole. You need the drawings that actually define the parts, in this case typically called "End Detail" drawings. These drawings typically show the two end sheets separately, so the details of the lap seam can be seen, and have numerous sectional views, both horizontal and vertical. Here is an example of the type of drawing you need:

NWHS NW-E48980-NW Mech Dwg

 

Unfortunately, the N&W H.S. archives does not have much on reefers.


Dennis Storzek



 
 


hockenheim68
 

 
Brian,

Glad to see you are still at it. When I've had the time to set it up (an all-nighter for me) I've been using CamBam for my CAM and loading the G-code into DeskCNC for machine control. DeskCNC has its own CAM program but I struggle to use it effectively - or at all. For what I'm trying to do CB is decent.  I use Dassault Systemes Draftsight for 2D CAD and Sketchup for 3D so you can tell what end of the spectrum I'm on. I'm not computer literate so what problems I've had are mostly down to lack of general computing knowledge. CB will do waterline, engraving and imports stl which is what I use for organic shapes coming out of sketchup. In my hands it is also much, much easier to use for general pocketing and contouring than DeskCNC which is the real bonus.  The latest version of CB has 40 free uses so it might be something you can try out. The old free version is buggy on the last computer I used it on (Vista, I think) and the Linux version is above and beyond my present ability to set up and use although I have heard good things from the few I've seen using it.



Andrew Hutchinson
Surrey BC Canada






grangerroads@...
 

Dennis, yep, your description of 2-1/2D milling is how I cut contours. To the touch, I can feel no ridges on the rounded surfaces I've cut, and they look great. I'll likely cut the Dreadnaught end from a block of machinable wax to ensure the tiny cutters don't snap all over the place.

My problem is how to CAD draw a square corner (early) 4/4 Dreadnaught end (is EDE correct?) so that I can extract cutting paths from it. I'll have to make an attempt from the 1943 CBC drawing, I guess, since I wouldn't know where to get an End Detail drawing of  the early 4/4. BTW, thanks much for helping me out, always much enjoy reading about your model-making processes. I learn a ton from your postings.

Andrew, CamBam, I will take a look at it. I've got FlashCut hardware and software for machine control, works great for me. Just now checked . . . FlashCut expects to offer a 3D version "soon." Among the offerings on its page are Rhino Cam. Since I have Rhino CAD, maybe I should break down and get Rhino CAM. Hate to see what it will cost. And what it will cost in time learning.

Sure do appreciate your mentioning CamBam though, thank you much.

Brian Chapman
Cedar Rapids, Iowa


hockenheim68
 

Dennis,

With one of these car end moulds, after you were done mopping up in the XY did you polish afterwards using a variant of the original tool paths? I've never seen a mould or pattern polished and I'm curious how it is accomplished when it is needed. Is it a matter of ramping into the work and in effect preloading the headstock a tenth or two  while the machine does its magic or something else altogether?

Thanks for your input thus far.

Andrew Hutchinson
Surrey BC Canada


destorzek@...
 




---In STMFC@..., <hockenheim68@...> wrote :

Dennis,

With one of these car end moulds, after you were done mopping up in the XY did you polish afterwards using a variant of the original tool paths? I've never seen a mould or pattern polished and I'm curious how it is accomplished when it is needed. Is it a matter of ramping into the work and in effect preloading the headstock a tenth or two  while the machine does its magic or something else altogether?
===============

I don't, but I'm not sure that directly answers your question, Since I cut very little directly into the cavity. Maybe Brian Leppert will take a stab at this, as I believe he does more 'hard milling'.

We are mostly an EDM shop (Electro Discharge Machining) so what I'm actually cutting are graphite electrodes that will be used to "sink" the cavity through a controlled erosion process. While the process is designed to erode the steel, it also erodes the graphite, albeit much more slowly, so that tends to obscure the tool marks. The process also leaves a consistent matte frosted finish on the steel.

Any surface that needs a higher polish for release purposes is "benched", polished by hand starting with diamond files, on to fine stones, and sometimes continuing with diamond polishing compound.

The same holds true with cavity work that is cut directly, which in our shop is mostly aluminum. This material is sufficiently soft that the diamond files aren't needed, but fine stones make quick work of the tool marks.

Dennis Storzek


caboose9792@...
 

 
 
In a message dated 1/29/2016 10:22:04 P.M. Central Standard Time, STMFC@... writes:
I don't, but I'm not sure that directly answers your question, Since I cut very little directly into the cavity. Maybe Brian Leppert will take a stab at this, as I believe he does more 'hard milling'.

We are mostly an EDM shop (Electro Discharge Machining) so what I'm actually cutting are graphite electrodes that will be used to " ;sink" the cavity through a controlled erosion process. While the process is designed to erode the steel, it also erodes the graphite, albeit much more slowly, so that tends to obscure the tool marks. The process also leaves a consistent matte frosted finish on the steel.

Any surface that needs a higher polish for release purposes is "benched", polished by hand starting with diamond files, on to fine stones, and sometimes continuing with diamond polishing compound.

The same holds true with cavity work that is cut directly, which in our shop is mostly aluminum. This material is sufficiently soft that the diamond files aren't needed, but fine stones make quick work of the tool marks.

Dennis Storzek
Only thing I have to add is we use hand held die grinders to do any touch up at work. Most of out die work is contracted out but we do occasionally do our own die repair at work, as well as we do change some parts of the die which ware down or fail with an accelerated rate. With a new die we run some test shots see how it runs and material flows and look for any marks in a finish surface. Any problems are marked depending on work needed from hand polishing to getting hit with the die grinders.

As the original poster wanted advice as to cutting dies for freight car ends having most or all the work EDM cut is the way to go. The first cost maybe high but you might see if a small local shop has the capability particularly if you have the work done as a low priority or "free time" project between regular orders for shops wishing to keep their machines and staff busy. depending on what your cutting and the tooling there is the matter of tool wear. As the tooling runs it physically wares down and looses its sharpness pushing metal rather than cutting it pushes a bur  of metal out of the way that is more bent over than cut.


At our shop part of my duties is to verify the machine operators gages are in spec and taking the measurements to assure the ware is being compensated for as the part is machined. So another step maybe to have pauses in the program or brake it into steps so you have the opportunity to stop and check the tooling and machine. Its easer to go back a short distance and recut than try to figure out were to go back a few hours or a day to redo a cut.

My final bit of advice is if nothing else go slow with the feed rate running at the max or close to it over the length of the cut is usually not worth the trouble particularly on a new program or one that needs to be  all it does is get you in trouble faster. I've never herd of any project coming in better than planned by over speeding but plenty that have gone bad, not only in quality of the cutting but also damage to the machine it's self.
 
Mark Rickert


hockenheim68
 

Dennis, Mark,

Thanks to both of you for your insight, it is very useful information.

I'm at the other end of the spectrum doing HSM stuff in the garage and at the kitchen table. So far the CNC rig, when run, has mostly been pattern making in wax but the goal is to produce some small usable moulds of N gauge stuff (ends, roofs, knuckle busters, etc.) to shoot in a small home-made injection moulder for personal use. EDM looks very interesting (seen the machines but not in use) and at about the time I made the IM I looked into making one of the more  popular homebuilt versions but concluded it to be beyond my abilities at present and possibly not really the right machine for the type of cavity I wanted to produce. There was some talk about the erosion on that particular design leaving surfaces that might need significant finishing after the fact which is sort of self defeating for my purposes. I think I can make something simpler for just burning out broken taps/tooling in and around the shop.
Mark's comments regarding blunt cutters and geometry are duly noted.  My home-made T/C grinding setup is incomplete and wouldn't work for small cutters  so I have to either buy new all the time for the CNC or back off silver steel specials in what amounts to a boring head and live with whatever it is I've made - something I  already do when working manually.

Thanks again for your help.

Andrew Hutchinson


grangerroads@...
 

> . . . a small home-made injection moulder for personal use. <

Andrew, did you work from plans to build your IM? Do you have information you wouldn't mind sharing? Thanks.

-Brian Chapman
Cedar Rapids, Iowa


hockenheim68
 

Brian,

E-mail me at hockenheim68atyahoodotcom and I'll show you what I made and what it was based off of. I've forgotten how to direct message from within the groups so this will have to suffice.

Andrew Hutchinson


---In STMFC@..., <grangerroads@...> wrote :

> . . . a small home-made injection moulder for personal use. <

Andrew, did you work from plans to build your IM? Do you have information you wouldn't mind sharing? Thanks.

-Brian Chapman
Cedar Rapids, Iowa