Machining snowboard base outlines

[3dcad]

I am a mold designer and I export files in iges format to a company that builds snowboards. They are new to the mastercam arena. The molds are machined flat and then formed in a press to put the radius of the tip and tails in. I have figured out how to scale the tip and tail shapes so when they form the mold, it comes back to the correct length. The tip and tail shapes are originally made up of 3 or 4 tangent arcs so when I unidirectionally scale the arcs out they turn into conics. I then make a spline out of the conics and convert them back to arcs. What this does is make allot of smaller arcs to follow the scaled out tip and tail.

The customer is buidling their own bases to fit into the molds that were built and is complaining that when they do toolpath, they get a bunch of little straight line segments instead of a real smooth toolpath around the tip and tail. Since I have no idea about the machining end of things, I am no help to them about solving the problem. They are using a cnc router to cut the bases to fit in the mold. The customer says that the toolpath moves to what appears to be the end of the arc and dwells for a moment and then moves to the next position and dwells. The result is a very segmented looking shape.They are rookies and this and are blaming my geometry as the culprit. I don't think this is the case because the company that makes the molds doesn't seem to have any problem. They don't want to help since they want to do the work for the snowboard company instead of showing them how to fix it.

 

Are there any switches that have to be set for importing the geometry or could they be running their feed rate to fast or could there be some kind of problem with the post processor? I have no idea and can't help them. I believe that they have level 2 Mastercam. I think that this may be a case of just not knowing how to use the program correctly but maybe someone can give me some insights into what direction to go into solving their problem. Thanks

[Zero]

That sounds like the controller or the machine to me... maybe change the gain or corner rounding on the controller? I don't know what feed rate they are running at, but that could also cause this to happen. I could be wrong, but I vaugely remember our first couple of parts on our first machine being like this and that's how we solved it.

 

You couls also try using the filter to make some of those line moves convert to arc moves.HTH

 

[ 08-14-2002, 04:34 PM: Message edited by: Zero ]

[Marker]

Sounds like the machine controller is reading a G61 and decelerating at each move.

[ERIC14779]

What is the make and model of the router that they are using?

 

If it is a Techno or a router with a Ah-Ha design group stepper control. I have seen our Techno with the MAC control and our other Techno with a Ah-Ha control do this...

 

It apears that it is due to a computer speed problem. I have a 200 Mhz pentium driving our Ah-Ha system. It has to calculate the next move. then do it,,,

 

[ 08-14-2002, 07:35 PM: Message edited by: ERIC14779 ]

[3dcad]

I believe the router is a Veisee Rover 321. Is there any kind of setting that can be changed as far as accuracy or curve tolerance on the igs imports?

[ERIC14779]

3dCad,

 

What CNC control does it use.. I have never heard of this brand.

[ERIC14779]

Also have them zoom in on the problem area in MasterCam and see if the same lines are there in the geometry that they are generating cnc code from... If it is you will not be able to get any better than the geometry you are using.

 

what software is used from start to finish to create this part... starting with what you are using, what accuracy you are putting out to their MasterCam seat ect.

[ERIC14779]

Just looked at Beisee's web site looks like they have a propriatary(sp) control I could not see if it excepts standard G code.

 

But my thinking still is that the geometry that MasterCam is working with has the flaws in it and is just passing these flaws on thru to the part.

 

Please check the accuracy if the geometry at each software before you convert to the next to see where it is going bad.

[3dcad]

The geometry was built in Cadkey. I checked all the geometry. They are tangent arcs and they import fine into every software that I have imported them into. Solidworks,Pro-E, Rhino3d.

 

[ 08-17-2002, 02:26 PM: Message edited by: 3dcad ]

[ERIC14779]

3dCad,

 

can you get some of the code that is sent to the router and post it here on the forum so we can see what it looks like??

 

Especialy the code that makes the bad surface

[David S]

quote:

---

the company that makes the molds doesn't seem to have any problem. They don't want to help ...

 

Are there any switches that have to be set for importing the geometry ...or could there be some kind of problem with the post processor?

---

Your geometry and post processor might be all good. Try some toolpath setting.

 

If they cut contour, try set Linearization tolerance higher.

 

If they cut a surface, try set Cut tolerance higher.

 

CNC machine works with a NC file. Inside NC file you may see: from point X1, Y1, Z1, (C1) to next point X2, Y2, Z2, (C2). That is a straight line. Shorter the line you make, smoother curve you will get.

 

Hope this will help.

 

PS. If I were you, I would give this project to the company that "doesn't seem to have any problem"(sounds like they want to do it} not some one "They are new to the mastercam arena". I will pay more to people with experience.

 

My design is not a high school science project, why give it to a student driver.

[David S]

quote:

---

They don't want to help since they want to do the work for the snowboard company instead of showing them how to fix it.

---

I would do the same thing!

 

I spend money sending my guys to James Class to learn some dirty secrets. Came back they crashed my best CNC. Finaly they could do MasterCam right.

 

Now, you want my guys go to the "student" company " showing them how to fix it" for free?

 

Ask MasterCam programers in this forum what do they think.

 

PS: I do not like the idea that use this forum hurting another MasterCam user. There may be many doing it. Then, please, do not tell us the story.

 

[ 08-18-2002, 12:41 AM: Message edited by: David S ]

[gmenzies]

you might suggest them to use there arc filter setting's in mastercam . if your cut tolarance is .001" heve them set it for .0012 . if you are

going for a higher tolarance .0001" then have them set it for .0003" , this will fit arcs where the geometry will allow . but unless there control can handle arcs ( mabey a cheap router )

then it will always be incremental moves.

 

Good luck

 

if you can upload the cadkey file . we used to use cadkey allot or upload the iges file .

 

[ 08-17-2002, 11:46 PM: Message edited by: gmenzies ]

[David S]

quote:

---

( mabey a cheap router )

then it will always be incremental moves.

---

That might be the problem.

 

quote:

---

a company that builds snowboards. They are new to the mastercam arena

---

3dcad, did you ask them what software they use before MasterCam? Did they have same problem like this before? How did they deal with it? Would you ask their MasterCam programer post his question and his setting up on this forum? He might give us more info. than you.

 

quote:

---

...my geometry ...the company that makes the molds doesn't seem to have any problem.

---

Please upload your geometry file and tell the programer give us his MasterCam file. We can start from there.

 

[ 08-18-2002, 01:04 AM: Message edited by: David S ]

[mold100]

Is it possible that the contoller is older technology and maybe doesnt have a very good look ahead feature and is simply not getting the information fast enough?Or if they are drip feeding at a low baud rate?Routers are not my line so sorry if I am not making sense.Just an opinion.

[Glenn Bouman]

I have worked with Biesse routers. The default cutting mode is G46 which does a complete stop between moves. Change that to a G47 and it will run smoothly.

[David S]

Bob (3dcad),

 

Thank you for the IGES files. Sorry did not get you back earlier. Monday morning, you know.

 

Look at the files; I would say the geometries are good, even though they are a little odd (8" long curve with 6 tangent arcs). I did a simple tool path on the problem area and gave it to the shop. The result is very nice. It is not like the company told you:” that the tool path is a bunch of little straight lines at this point".

 

If this is only area had problems, then their controller is good. It can handle arcs.

 

At this point, I do not know what to say without look at their .mc9 file.

 

There are two things you could do might help them solve this problem:

 

1. Tell them to slower feeding speed, use sharp tool and use Multi Passes feature (set finishing pass to 0.02). Do not use Highfeed feature.

 

2. If their controller could not do little arcs (G46, G47 dose not work good), please give them a Spline instead 6 little tangent arcs. Tell them to set Linearization tolerance higher when do the tool path.

 

Hope these will help.

 

[ 08-19-2002, 01:27 PM: Message edited by: David S ]

[3dcad]

Guys, Thanks for all your help. I will leave this in their hands and let them deal with the fine tuning end of their programs. I think they have figured out some things with all of your help.

Thanks again.