Page 3 of 3 FirstFirst 123
  1. #21
    Charlie, I did read this a while ago and do have some comments.

    Firstly is understanding the problems created by the drawing/design. Cad means you can draw anything these days but that doesn't mean you can make it easily if at all in some cases, also vs cost of the designed part as apposed to a re-design that will do the same thing but is far cheaper/easier to produce. These are wise words worth heeding to anyone who is a little green. Get advice from someone who actually knows what they are doing, who ever it is.

    It's a big problem for guys like me in the trade where we constantly get drawings from people who are not trained/ brought up in the trade this also includes so called professionals at times. Someone taught them how to use cad at some point (including universities and colleges) with no understanding of manufacturing The only proper transition is from the shop floor to design, often with only a few exceptions these days. This is the only way people learn how to design properly. This is becoming a huge, huge problem for people like me now and it is all but costing me my living by having to advise and sort designers lack of knowledge/ability unpaid, consuming hours of my time every week. Understanding the cause of the problem helps you find a solution for the future.

    Sadly this will never be addressed properly in the Uk unless we go back to being a proper manufacturing nation using old school methods of learning.

    Understanding the above comments would have helped you with your part.

    The small square shoulder at one end of the part is the problem as you now know from others. So you have to design around that problem. Is it doable as it is.... hmmm yes probably but it makes life difficult and expensive, so look for an easier solution, put a rad where that square shoulder is so its a transition from one square to the next, this will allow you to 3D the rad and gets rid of the square corner problem. You would have to use a small ball nose (explained later) lets say 6mm so put a 3.5 rad in that corner so there is no collision of cutter rad to part rad. If that square corner is used as a stop then put a small pin in place of the stop, it will do the same thing but far cheaper and easier.

    The other very obvious solution is the turn the part on its end and machine in that orientation the square corner then becomes a non problem its a simple 2d path on a cnc. Not having dimensions I have no idea how long that step is or if its to long to do in that orientation. Information is power provide people with more info then they are better equipped to help you.

    The rad on the edges is something that needs to be considered, (assuming rad cutter is out of the equation due to size and cost) because it's 25 mm square with 8 mm rads, that means in real terms when you come to do the last set of rads you have 25-8-8 which leaves 9mm of flat left to hold on, this is fine for the first 2 rads but lets say we are going to use a 6mm ball nose for finishing. The cutter will be at the furthest point from the ball at the lowest part of the rad being machined this then leaves 9mm-6mm this gives you 3mm to hold on plus you need some clearance for the cutter so 2 mm to hold on... not a lot! This is based on a machinist who would naturally look at a vice/vices as the cheapest and easiest option to hold the part.. a smaller ball nose will give you more clearance but you sacrifice rigidity and of course more risk of breakage with smaller cutters. The obvious solution is 2 tapped holes in the part either end and a plate with 2 back stops (dowels) to clamp the part to, either leave the job long and clamp on the ends and cut that off later and machine, or two tapped holes to clamp through the plate or a variation on that theme. This method leaves you with 9mm + 8mm = 17mm of free space for the ball nose to do its job. Tons! Plus you can now use a bigger ball nose for better cutting and more rigidity.

    Lastly, the machining process you have used is wrong. With this part you would:

    1] Do the rads first.
    2) Holes through the V (in a vice for ease)
    3) Only then would you do the v cut out (in a vice) with the part being machined supported in the vice and not extended out from the jaws.

    The reasons are as soon as you cut out that V you take away support and rigidity from the part to do the rads this means deflection caused by the V having the material machined away, This is about good standard machine shop practices and getting into good habits and understanding the processes a machine shop guy should employ.

    Yes you would natural machine the rads along its x axis (omitting the step as it is) from left to right or right to left with the z and y stepping progressively is your software will allow this machining strategy. Rough first then finish with either a ball or bull nose. A bull nose would help would help with the clearance issues if trying to hold the part in a vice to produce the rad

    Regarding the guy that did the work. Sorry if you managed to find one of the non competent ones out there, some of the issues i raised may well be why you have not had a complete job returned, but the bottom line is, he charged you nothing and if you pay peanuts.... well sorry to say you got monkeys. What he charged you would cost me more to keep the doors of my works open for the time the job would take.. ie I would lose money.

    We have dealt with each other before charlie as you know and nothing is said with malice I'm just being straight, nothing personal.

    All the best.
    Last edited by spluppit; 6 Days Ago at 07:30 PM.

  2. #22
    I have done a way with the step now to simplify it so its just the 8mm radius I'm stuck on which I cant really get rid off. It slots into something on one end and something else slide over it and is located in the center.
    I have been trying to figure the cam out on fusion360 but haven't found the right strategy yet. if anyone who uses fusion has any tips it would be great.

  3. A quick look suggests to me that Adaptive Clearance with Contour Finishing might get you where you want to be, Autodesk documentation isn't the greatest though and I'm a BOB-CAM user.
    You think that's too expensive? You're not a Model Engineer are you? :D

  4. #24
    I'm with M_c (post #19) on this.

    Clamp the bar in a V-Block held in the vice and mill each corner off the square one edge at a time (fliping/inexing the bar over in the V-Block for each edge and only mill as far as the step needs to be), to in effect give you the octagonal shape you first thought of, where it goes into the other tube.
    Set an end stop for the bar to butt up to and use the end of the cutter not the side.

    There's other methods, but this is the quickest (if youve got a big enough V-Block) and easiest with limited equipment.

    Last edited by Nick952; 6 Days Ago at 10:25 PM.

  5. #25
    cheers I think I have managed to get a tool path sorted so will give it a test tomorow

Page 3 of 3 FirstFirst 123

Similar Threads

  1. Matching a radius
    By kell in forum Solidworks
    Replies: 2
    Last Post: 01-12-2015, 11:18 AM
  2. Machineing horns.
    By simonms in forum Machine Discussion
    Replies: 0
    Last Post: 05-02-2015, 11:47 AM
  3. Hole Radius
    By benkat in forum Machine Discussion
    Replies: 0
    Last Post: 03-03-2014, 05:29 PM
  4. Replies: 0
    Last Post: 10-06-2012, 07:59 PM
  5. Ragged edges
    By Minnican in forum Machine Discussion
    Replies: 14
    Last Post: 25-04-2011, 02:32 PM


Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts