Surface flowline help

[Lars Christensen]

Hi guy's

Let me start out saying that I am totaly green in surface milling, fact is that this is my 1st. piece.

I have upladed on cadcam's FTP a file in the Mcam8 folder called "Lars surface".

If someone would take a look at this file and give me some advice it would be highly apriciatted.

What I did was creating 5 surfaces using sweep, and after reading here on the forum I desided using flowline. Now I would like to haved runned a ball endmill, and then using a flat endmill to take radius's out were needed, I was thinking of using "left over" but I never came that far, because I realized that the ball endmill would cut under my lower surface line to creat the surface. (Making any sence?) so I thought if I created a flat surface .03" around my already surface, the ball would stay above, but then it told me that there was issues with the flowline toolpath.

What I ended up using was a flat endmill with .0005 step, it got the job done, but I know it is not the right way.

I would verly apreciate if some of you could give me some help. Maybe I sould have used something else than sweep to create surface, or maybe flowline was wrong

 

Thanks

Lars

(who walks in the dark world of surface)

[Jack Mitchell]

"I realized that the ball endmill would cut under my lower surface line to creat the surface. (Making any sence?) so I thought if I created a flat surface .03" around my already surface, the ball would stay above, but then it told me that there was issues with the flowline toolpath"

 

Make the flat surface all around but make this larger by say about a 1/2" - this you will call a check surface (Which means that a tool will not violate a check surface) this could have also been done on your upper surface as well.

Play with these features some more so as that you will understand surfacing a litle better.

 

Delete the operations with your operation mgr and try again - follow the prompts and this will come.

 

 

Not a bad shot for a first-time attempt

 

Regards, Jack

[DavidB]

Lars,

 

I took at look at your file.

Anyalize/sufaces/check modal /all surfaces you will see you have 4 surfaces with sharp internal corners.This is common with with sweept surfaces that have a sharp transition.

 

Im not sure what shape you actually wanted but the walls are a straight surface should they be a rad?

 

As for the tool path what you did is fine.May be you could have used a ballnose?

 

You could also have done the Machining with a surface finish contour.A boundery would be needed to keep the tool on the outside of the surface though.

 

HTH

[Scott Bond]

+1 Not a bad shot for a first-time attempt .

Jacks .02 is a good way, you could also fix what you have by useing the Trim feature on the unwanted cuts .

[DavidB]

Also,

on the last page of the toolpath tick Deepth and set the Max deepth to the height you want the tool NOT to go past.

 

[Jack Mitchell]

All responses are fair concerning this project.

For me - I always use flat boundry whenever possible for defining the upper or lower surfaces because to me this is the most direct approach giving you exactly what you need to get the task done. (shading and zooming will tell the true condition) As I said, play with this application because it is simple and it is an excellant learning tool within itself.

 

P.S. There is probably a half dozen different ways to approach this task. Many people use boundries and containments - I rarely do - but it's really a personal choice given everybody's own particular experience or discipline.

 

 

Regards, Jack

[Don S at Barefoot CNC South]

Lars

Check out the file I did in FTP I used contanment boundries as explained also used contour tool paths.

 

HTH

 

Don S

[Lars Christensen]

Thanks so much guy's you are the best.

 

Jack,

I tryed your way, and it worked right away (Knew that check surface had to be there for a resaon )

 

DavidB,

quote:

---

Im not sure what shape you actually wanted but the walls are a straight surface should they be a rad?

---

No, somehow I actelly got the surface created the way the customer wanted it:D It is a coin insert for a die.

quote:

---

You could also have done the Machining with a surface finish contour.A boundery would be needed to keep the tool on the outside of the surface though.

---

I tryed this but have problems getting the front face (.02 rad going to a 20 degree line and then into a .04 rad.) milled.

 

Scott,

Trim surfaces is something I have to sit down and take some more time on. I cant for the life of me figure out how to control the arrow that desides what to be trimmed.

 

Don S.

Thanks for the file, I only wanted the outside milled (My mistake not closing up the geometry)

As I told DavidB I can not get the "front" face milled. What does it means when it turns red when you are regenerate the toolpath?

 

I verly apreciate all you guy's help, again I realize that Mcam gives you 100 different ways to do stuff, what is making this software great.

 

quote:

---

Not a bad shot for a first-time attempt

---

When you have found the "search function" on this forum, you have verly found the tool of your life

 

Lars

[DavidB]

Lars,

I opened your file did a surface finish contour with a boundary and using Deepth.

I went to save it as a MC8 file for you just so tou could have a look and MC said it will only save Geometry not Toolpaths

 

Im using MC9 sorry.

[Phil Orenstein]

I went to school on this one myself. One other method to contain the depth is to use depth limits where the bottom of the geometry is the maximum depth. Also I would use the Zig zag cutting method to avoid all those retractions, unless you purposefully want to climb mill that surface.

 

HTH

Phil

[Lars Christensen]

DavidB,

I am using Mcam 8 at work, but I have the Mcam 9 demo version here at home. So unless you deleted the file, I can see it. (dont want you to go over your trouble twize).

Got to go and get some sleep though, thanks again.

 

Lars

[Lars Christensen]

I got to try to play around with those depth limits.

 

Phil,

quote:

---

unless you purposefully want to climb mill that surface.

---

I thought (not being a smart xxxx!! milling is new to me) that you always should use climb milling on a CNC-Mill, for finish and tool life.

 

 

Another thing I might should add, is that this block was rework, 1st. the customer just wanted a straight island standing, later he added the rads. and tapered walls, so I just had to take a small amount off.

 

Lars

[DavidB]

Lars,

 

I put your file on FTP site in MC9 folder.

Check out level 200.

 

HTH

[Mike Whitten CAD/CAM Contractors]

Lars,

 

I am glad that everyone has helped you out here so I will not have a look at it but I will comment on the "Red" thing.

quote:

---

What does it means when it turns red when you are regenerate the toolpath?

---

I have always had this problem but have not consulted CNC software yet. I believe it to be a Bug. What I do is just save and exit and then just Re-open the file. I have not had it affect my code. It is just an annoyance.

 

Thanks,

Mike

[Lars Christensen]

DavidB,

I got it, I was making the boundery at the bottom of the surface, makes sence it have to be at top, and now I understand what the depth function does. Thank you so much for taking the time.

 

Phil, Anybody, a comment on the ZigZag compared to One Way, is it because you normaly isent taking very big cuts, that it has no effect on finish and tool wear?

 

Michael,

Thanks I will not worry about the "Red" for now.

 

Thanks for the help.

 

Lars

[DavidB]

Lars,

 

The Boundary doesn't matter if it is any where in Z axis Mastercam looks at the boundary through the C/plane so it makes no differance where in Z the boundary lays.

 

Zigzag will give you climb and upmilling but would keep tool on job.Doing a finish pass on a small erea like your job would not matter to do Zigzag.

 

The one thing that i would do is extend the sufaces so they go past the erea of material.So as the tool retcacts and returns to job it's not actually on the workpiece.Just so you dont get any dwell makes.

 

Generally you are correct and climb milling is first choice.

 

HTH

 

[Lars Christensen]

DavidB,

I can not get it to do it as countur if I make the bondary at the bottom of the surface, it will not machine the long surface.

I have gotton a alarm called"Internal sharp corner test" once and awhile.

 

Lars

[Lars Christensen]

DavidB,

quote:

---

The one thing that i would do is extend the sufaces so they go past the erea of material.So as the tool retcacts and returns to job it's not actually on the workpiece.Just so you dont get any dwell makes.

---

I did that. I should had included the STL file from prevuis run. That would have made it alot eaysier for you guy's.

 

Thanks for making the Climb, ZigZag clear for me.

 

Lars

Foster

[DavidB]

Lars,

 

Try this with the boundary in the toolpath you got to work.Xform the boundary in Z to any where you like.Regen the Toolpath this will show you its not the boundary thats the problem.As i said in preverse post your surfaces have internal sharp corners thats what MC is alarming on.

 

HTH

[Lars Christensen]

DavidB,

 

You are right I just translatet the upper blue geometry you created for the bondary down, and now I dont have a problem using the surface contour. I must have messed something up when I tryed last night.

 

Thanks for all your help. I will be playing with this surface stuff some more, and probely come back with some more questions here on the forum.

 

thanks

Lars

[Phil Orenstein]

Another comment on the zig zag Lars. I use climb cutting (clockwise on OD cuts) whenever I can except on surface cuts like the flowline and surface contour where climb necessitates one way cutting. To avoid all the retractions, I ususally use zig zag. The finish is theoretically better usin climb all the way, but the step downs typically used are so small that it doesn't really matter. As I understand it (correct me if I am wrong) climb pushes the cutter away from the stock and conventional pulls it in. But with tiny cuts it doesnt ammount to much.

 

Phil

[billystein]

Hey Phil

From the spelling on this topic. I'd say you are the only one here that went to school

[Teh Bear without Brains kinda idiot]

~~~~~~~

From the spelling on this topic. I'd say you are the only one here that went to school

~~~~~

Me supposes it are the jocke .

If it aer the jokc ,you must adde J/k or

I hoppes it are notte offensse .

 

Teh spell on you

[DavidB]

Billystein,

 

If someone is helped in thier querry who cares what the spelling is like.

This Forum is for helping others and getting help not putting other people down

 

Maybe one day if you have question and are seeking an answer you will reply to whom ever helped you "Thanks but next time get the spelling right?"

[Lars Christensen]

Thanks Phil,

I thought that was the reason for the zig zag.

 

Billystein WHY???????

 

Lars