Surface Mill -- Flowline Problems

[Beck]

Has anyone experienced problems with the Flowline operation? I use negative stock while cutting electrodes, and the tip of the cutter doubles the stock value. If I say -.005", it cuts my electrode .010 undersize. I was told to use "Center" rather than "Tip" in the "Tip Comp" menu. I really do not want to change to "Center". If they fixed it in 9.1, let me know!

[kyle]

Saying -.005 will remove .005/side off a dia. If you had a 1.000 dia. it would then cut .9900.

[Guest CNC Apps Guy 1]

Kyle is right. Flowline is doing exactly what it is supposed to be doing.

 

JM2C

[MLee]

I guess I'm a little confused, if you are cutting a round piece then it would double becouse it is "per side", but if you were just cutting 3D surfaces I don't think it should, or at least I hope it shouldn't becouse I do this all the time with the molds I work on, I cut it, they run parts, then sometimes they tell me to take some material out of some places. If this is true then I always take twice as much as the engineers tell me to??

[Guest CNC Apps Guy 1]

The value of stock to leave is "Per Side". So if you have a boss and you need it .005 under (the boss that is), then your stock to leave is -.0025 and theoretically you should be where you think you shoud be. But, if you're doing a sculpted surface ans you need it to be .005 under, your stock to leave is -.005.

 

HTH

[Guy Arseneault]

I had the same problem. It would cut ok going down the sides but when it came to do the radius it took double the amount.I've loaded a file called flowline.mc9 in the mc9 folder.It has 3 toolpaths with no negative stock, minus .003 and minus .008.

 

Thanks Guy

[P_Scott]

Beck,

 

BTW, welcome to the forum. If you are surfacing a "U" shape cavity (hypothetically), and tell it to leave -.005" for stock, you will be removing .005" of material past the left-hand side of the "U" and .005" past the right-hand side of the "U". This totals to an overall size difference of .010" You could also Offset the surfaces the amount of stock you wish to remove and cut them again, with 0.0" stock to leave value.

The tip comp will simply produce toolpath calculated from the Tangent point of the ball (Tip comp) or the center point of the ball (Center). If using tip, the toolpath will look like a parabola (bell curve) from the side. If using center, the toolpath will be a radial offset of the surfaces. Center essentially allows the user to change the size of the tool and offset the toolpath, without re-generation of the toolpath in Mcam. HTH

[Dan Bedore]

hypothetically), and tell it to leave -.005" for stock, you will be removing .005" of material past the left-hand side of the "U" and .005" past the right-hand side of the "U". This totals to an overall size difference of .010"

 

Won't you also remove .005 from the bottom of the "U".

[P_Scott]

Dan,

 

You are correct. You will be removing material from both sides and the bottom. I used the "U" shape to try to simplify the explanation, seeing as I didn't have any geometry to base the example on. The point is that the -.005" stock to leave is for making the overall size of the cavity .010" larger from side to side, but only .005" deeper, or like offsetting the shape of the "U" by .005" all around. I hope this clarifies things further.

[Guy Arseneault]

Peter,

 

I tried your example and it does what Beck said,

at the bottom of the "u" it goes double the negative stock. I don't know if you saw my post but I loaded a file that does the same thing.

 

Thanks,

Guy

 

[ 01-23-2003, 01:34 PM: Message edited by: Guy Arseneault ]

[Dan Bedore]

guy how did you tell that it went twice the distance. just woundering how i can check a cut path with out cutting a part.

[Beck]

To All,

Thank You for responding today.

 

Guy, I see that you also experienced the same problem. It is at the bottom of a U-shape that the cutter doubles the negative stock. Thank You Very Much.

 

To clarify to everyone, I am getting the proper results on the sides of a U-shaped cavity. BUT, at the bottom of the cavity, I am getting the ball cutter to exceed the desired shape by 100% of the negative stock. If I want the bottom to be -.005, it is .010" lower. This can be seen by producing a path and viewing it in the front view. Take a snapshot and measure all you want. Also use the same settings using "Parallel" rather than "Flowline". you can see the difference. I have been using this properly in V8 for years and finally switched to V9.0 Now it fails.

To repeat my original question concerning V9.1...

Does the Beta version fix the problem?

[Glenn Bouman]

Put your file on the ftp site so we can check it out. I tried your example with 8.1 and 9.0sp1 and 9.1 and the results are the same.

[mold100]

I have frequent flyer miles using flow to cut electrodes and have never encountered this,just curious why would you use center?,try tip and check your results

[P_Scott]

Beck,

 

Make sure you have all the latest Surface Toolpath Apps patches. The last one was dated 10/15/02 but was actually released in Dec. Another option would be to try a different toolpath. The Surface-Finish-Project-Blend-3D seems to work well as a Flowline replacement toolpath. Flowline was never really the best toolpath for multiple surfaces. Finish-Scallop for example, when applied to your part with the settings for -.008" stock, does only take the amount to leave value off the surfaces. Look at all your options. HTH

[Beck]

Mold 100,

 

I have always used "tip" only. I was told to use center to fix the problem. It is the work-around! But with center, I have to pick up all my tooling differently.

 

Please do this for me. (I have experienced the problem with even a flat horizontal surface.) Create a surface at Z0.0,

Set your stock at -.005, and tell me what depth your cutter ends up at. My path is at Z-.010.

[mold100]

I just created flat surface and flowed it to -.005

and it backplots correctly using tip.When I use

center it does some funny things multiple passes?? But using tip worked alright.

[Guy Arseneault]

Beck,

 

quote:

---

Guy, I see that you also experienced the same problem. It is at the bottom of a U-shape that the cutter doubles the negative stock. Thank You Very Much.

---

quote:

---

Peter,

 

I tried your example and it does what Beck said,

at the bottom of the "u" it goes double the negative stock. I don't know if you saw my post but I loaded a file that does the same thing.

 

---

Dan Bedore

quote:

---

guy how did you tell that it went twice the distance. just woundering how i can check a cut path with out cutting a part.

 

---

By backplotting in the front view.

 

Guy

 

[ 01-24-2003, 11:55 AM: Message edited by: Guy Arseneault ]

[Beck]

Mold 100,

I wonder why it is working for you and not for me?

I have loaded the latest patch.

Thank You for your time. It has been helpful.

 

Anyone else who tries the Flowline test, please let me know the results. I will check the BB 2-3 times a day.

 

Beck

[Dan Bedore]

so Guy are you saving the cut path as geometry and then measuring?

[mark l]

I tried the flat surface deal and it worked fine, I posted it out and Z went to -.005, I also saved toolpath as geometry and measured that and was also -.005. But here is the funny thing, I tried it first with a flat end mill and it said "radius on tool can not be smaller than neg. stock"?? I thought that was kind of odd. Anyways just my 2CW

[mold100]

mark l,

You cant cut negative stock with a sharp endmill when surface cutting,you need a radius on the corner minimum of the negative stock.

 

ex. to cut this you would need to tell it the cutter is a bullnose with .005 or maybe .0051 corner radius.

 

Hope this helps.

[Guest CNC Apps Guy 1]

quote:

---

But here is the funny thing, I tried it first with a flat end mill and it said "radius on tool can not be smaller than neg. stock"?? I thought that was kind of odd.

---

The problem lies in being able to calculate a tangency point on a sharp tool. That's why Mastercam has a problem with this as of now. Perhaps they will find a solution but as of now, you need to have a tool with as much corner radius as you want to cut negative.

[mikhael gutman]

Hi Beck!

I am usually “lying” on diam. of cutter on 2 orbits. So if your orbit 0.003 and cutter 0.06 – program for diam. of cutter 0.054 if you using spherical orbit and cutter ball.

For standard orbit you have to modify geometry or use flat cutter if it possible

[mold100]

Too much work there,mikhael, We've covered this

pretty thourough a couple of times try a search.

 

[ 01-25-2003, 09:38 PM: Message edited by: mold100 ]