3D

[Frank]

Hello: I would like someone out there who is an expert on 3D machining help me on this problem. Anyway I have a piston cad file...and I have a forged piston, the cad file I have is the way they want the piston machined. It's the back side and they're goal is to lighten up the part. Some places I'm only taking about .010 of stock off, other places as much as .200. The way I programmed it...I used the rough pocket surface program leaving .010 stk. and then used finish parallel @ 90 and 0 degrees

machining.

The problem is the pocket program cuts a lot of air, and air is time, and we all know what time is. How would a 3D experienced programmer attack this type of part.

Thank You,

Frank

[bstall]

Can you use boundries or depth limits to isolate the difference in stock thickness you are machining? I rarely use roughing strategies. You can get a closer to net shape if you rough using finishing strategies. You will increase the amount of operations but the result at the mill will be improved dramatically (that is what companies will see). There are many different ways of going about it, just stay open minded and don't feel you have to machine by the "standard" practices.

[Frank]

Are you saying to use finish paralell, and use depth cuts for the heavy area's of stock ? Please elaborate. And thank you for the response.

[KEVCAM]

Hi Frank,

I have had a fair expeirence with 3d programming and 4th axis rotational positioning 3d surfaces. I have strolled upon a possible glitch in the software with rough parallel surfacing.

First you have to squash the profile or geometry that conatins the 3d surface too a contruction plane that is 90 degrees to the surface. If you generate a rough surface toolpath and rotate the construction plane 45 degrees and leave the tool plane at 0 degrees; and of course set your max. and min. depths and depth increments and leave your 0.010" or 0.015" on for a finish pass (using surface parallel finish). You must also chain your profile as a tool center boundary at the 45 degree contruction plane.(Important key!!) You will find that it generates a toolpath that will be automatically trimmed to the surface controlled complety by using your depth limits. This will eliminate perfectly maching air.

It may seem confusing going through this the first time; but it works very slick.

Good Luck

------------------

Kevin Lee

CNC PROGRAMMER

UWO London, Ontario

Canada

[Lee.]

I'm no expert on 3d machining but have done a fair bit of roughing. Try this. Create edge curves and use the inside ones to squash to a different z level. offset this chain enough that your tool will go between this geometry and the part, taking in to account that you are leaving some stock on, so you'll be away from the part a little. Then create a solid extruding using this geometry. Then pick both solids when roughing out and you won't cut as much fresh air. e-mail me the file if you like, or have problems. You'll likely have to rough out the bottom of the pocket with out using this extra solid but can restrict the z moves and create an extra operation.Posting both together you'll get all the roughing done with the same program.

[email protected]

------------------

L.K.White

Premier Pattern Equipment Ltd

Edmomton, AB.

[KEVCAM]

CHALKYW

So you mean when offsetting the geometry to fit the tool bewteen it and the part, are you creating a tool center boundary? If you are you dont have to offset extra to leave material on. You can control it with your stock to leave on drive surfaces.

Can you explain a little better.

Thanks

------------------

Kevin Lee

CNC PROGRAMMER

UWO London, Ontario

Canada

[Lee.]

KEVCAM

What I was trying to acheive here was a solid body entity that acts like a tool boundary. Not to confuse stock to leave, that is controlled in the ops manager. When roughing out a part on the inside, mastercam will not accept geometry boundaries, so, you have to create the solid to stop the tool from unnecessarily going there. Please let me know if this works for you.

[Karl Oram]

Hi Frank

Because MasterCam is so versatile this problem can have so many answers all of them will probably work.

First you have to decide how much extra time it is taking when cutting air and how many of them you have to cut against how long would it take you achieve a more visually acceptable toolpath.

Many people chase their tale taking days to achieve the absolute perfect "Visual Program" when they have one piece to run and its done in three hours ?????

Anyway here is another option:

You have a model of the Correct Piston.

Model up or get the data for the Forged Piston.

Create an STL file of the Forged Data

Run a constant Z toolpath (Contour) leaving .015 to .035 (whatever is best for your set up)

Use High Feed To optimize the Feed Rate.

Use Forged Model STL file as the Stock.

This method will not only eliminate unnecessary air moves but will optimize the feed rates as they vary in amount between you .010 and .200.

Regards

Karl Oram

Caledonian CADCAM

Scotland.

[Kenneth Potter]

Ok heres another option.

Create your tool center boundrys above your part & if you like create multi TCB's to isolate troubling areas & lable then to different levels"layers. Now heres the fun part. Create tool path 2d pocket for each tool center boudry using the many tool path options, Make the Z final depth for each pocket incremental O . Then use rough project. Parameters tab, Cut tol, Max step down, Projection type"nci". Plunge comtrol "Allow multiple plunges along cut". This method has many options & flexibility's .And you will keep the assoativity active if you deciced to make minor or major changes using the regen option.

Kenny

[Frank]

Thank you all for all the responses Karl I'm trying to figure out what a STL file is, I see I have a converter for it, do I bring the file into Mastercam then write it as an STL, then what? I've used my help files on this subject and it wasn't very helpfull. If I could be able to do this it would be a great help. Our customer wants to use the same forging to try all kinds of different cuts on his piston.....and it sounds like using STL would be an answer. Actually I just learned that there is no "writing on the wall" to machine 3D from all the different responses I've recieved.......Thanks again.

Frank

[Karl Oram]

Apologies Frank

The STL was a wrong Steer ,I was thinking of my other CAM package DREAM CAM -

What you do is merge the CAD file of the Forged Piston Data.

Place into position relative to the finished part.

Place it on a Different level than the rest of the geometry.

Turn off all other levels except the Forged Piston Data.

Do Toolpath > Multi surface finish (Zigzag)and leave +.020 all over.

Now turn off that level and turn on the finished data.

Do a Multi Surf Finish Contour to Leave +.010 to +.025

So now we have 2 Toolpaths.

The first will be used to establish the Stock for the High Feed Calculation for the Second toolpath.

Highlight the 2nd Op in the Op Manager and select High Feed From the right hand side.

For Stock use the Scan NCI option to Look at toolpath #1

The other Values you set according to your machine if its the first time you have run this Feature set the Min and Max Feeds to your comfort Zones And Read the Help File.

It will calculate and modify Feed rate depending on the amount of material removal so where you have +.200 it would be slower than where you have +.010.

For more help you should read this Doc file (Hfapp_v8.doc) found here http://www.mastercam.com >>>> in the support > free download section.

Regards Karl

Caledonian CADCAM

Scotland

[Metal_Eater]

I would suggest following.

Finish machine your forging CAD file using parralell finish toolpath.

Now take your finished piston CAd file & use

TOOLPATH->surface-> finish Countour,

& click on REST MILL, set your required stepover & stepdown in rest mill page.Leave +.01->015" on. This will calculate exact geometry of material to be removed from previous operation.

Then create one more finish countour pass to make it to size.

You dont need to post the very first operaion as it was done only for calculation purpose.

Hope it will help.