Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

2021 swarf toolpath


cncasylum
 Share

Recommended Posts

Download my sample file from CamInstructor. I have a swarf toolpath in that example that might help. 

CamInstructor Link

Without a sample file to see what your seeing going to extremely hard for anyone to know how to help. Do you have a floor surface checked? Are you using upper and lower edges? Are you using tilt lines? What is the normal of the surfaces if using surfaces and not solids? 

Link to comment
Share on other sites
19 minutes ago, crazy^millman said:

Download my sample file from CamInstructor. I have a swarf toolpath in that example that might help. 

CamInstructor Link

Without a sample file to see what your seeing going to extremely hard for anyone to know how to help. Do you have a floor surface checked? Are you using upper and lower edges? Are you using tilt lines? What is the normal of the surfaces if using surfaces and not solids? 

Ok great thanks for feed bk. I need to learn how to poat a sample file on this forum. I will do that and post it in the morning. Ill check out your video. I loved your 1st couple. Im checking that one out now. This project has me stuck at work trouble shooting.

Link to comment
Share on other sites
17 minutes ago, cncasylum said:

Ok great thanks for feed bk. I need to learn how to poat a sample file on this forum. I will do that and post it in the morning. Ill check out your video. I loved your 1st couple. Im checking that one out now. This project has me stuck at work trouble shooting.

My Phone Number is on my website. Give me a call and I will see if I can help you solve it over the phone.

Link to comment
Share on other sites

Here is a sample file. I did swarf, but used 5 different methods. I prefer the use Tilt lines one that is the last toolpath, but they are driven from the same geometry and see how each one acts a little differently. A good way to learn these toolpaths is to do this very thing. Try things and see what and how they work.

5TH AXIS COMPLEX SWARF EXAMPLE download link

Have a good weekend. :thumbup:

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
10 hours ago, crazy^millman said:

Download my sample file from CamInstructor. I have a swarf toolpath in that example that might help. 

CamInstructor Link

Without a sample file to see what your seeing going to extremely hard for anyone to know how to help. Do you have a floor surface checked? Are you using upper and lower edges? Are you using tilt lines? What is the normal of the surfaces if using surfaces and not solids? 

 

CA-50-M009-20R1BLANK.mcam

Link to comment
Share on other sites
6 hours ago, cncasylum said:

Your problem was grabbing the radius as the floor surface. Only need to grab the walls and the one floor in that area. The toolpath will go to the radius. The radius is not .125 all the way around and the .002 difference in places and broken in other places are the problem. Nice work defining your levels.

Glad I was able to point you in the right direction.

  • Thanks 1
Link to comment
Share on other sites
19 minutes ago, cncasylum said:

JUST LEARNED THAT PLANES NEED TO BE TOP  AND TOP. THINKING THATS A T.C.P.C THANG.

No Planes need to match the WCS that is being used. If you have moved everything to TOP/TOP then yes your planes could be TOP/TOP, but 5 axis toolpaths will work regardless of the planes when doing 5 axis. The difference is the WCS is the Zero and orientation in which a programmer is making the programs. If the model is moved to Top then it could be Top/Front, TOP/Back, TOP/Right, TOP/Left and Top/Whatever plane you need and the 5 Axis toolpath will work. The WCS is what controls the output for the the program in relationship to how you are going to machine it on the machine. I have a part right now with 4 different Lathe Groups. It is a Vertical Mill/Turn part. I have one finish model and 4 Setups coming from that one model. It is about 800 operations and 12 tapes out of Mastercam. I currently have 4 WCS planes for each side and rotation of the part. I have another 40 planes for the other things going on.

Review the file on CamInstructor. I have a FACE1 WCS and then 4 other Planes for each face. The WCS for the operations doesn't match TOP. That was on purpose to help people understand the WCS process on a simple part like that.

FYI CAPS IS CONSIDERED RUDE AND YELLING so please turn off the caps lock when responding on the forum. Have a good day.

Link to comment
Share on other sites

That just all soun

On 11/14/2020 at 12:28 PM, crazy^millman said:

No Planes need to match the WCS that is being used. If you have moved everything to TOP/TOP then yes your planes could be TOP/TOP, but 5 axis toolpaths will work regardless of the planes when doing 5 axis. The difference is the WCS is the Zero and orientation in which a programmer is making the programs. If the model is moved to Top then it could be Top/Front, TOP/Back, TOP/Right, TOP/Left and Top/Whatever plane you need and the 5 Axis toolpath will work. The WCS is what controls the output for the the program in relationship to how you are going to machine it on the machine. I have a part right now with 4 different Lathe Groups. It is a Vertical Mill/Turn part. I have one finish model and 4 Setups coming from that one model. It is about 800 operations and 12 tapes out of Mastercam. I currently have 4 WCS planes for each side and rotation of the part. I have another 40 planes for the other things going on.

Review the file on CamInstructor. I have a FACE1 WCS and then 4 other Planes for each face. The WCS for the operations doesn't match TOP. That was on purpose to help people understand the WCS process on a simple part like that.

FYI CAPS IS CONSIDERED RUDE AND YELLING so please turn off the caps lock when responding on the forum. Have a good day.

That just all sounds insane. I imagine over time and constant improvement it is the destination. I've been machining and playing  with mills for 15 years , mainly vertical 2d applications. The last 3 to 4 have been pushing into 3d toolpaths. Just this past march boss man purchased an Okuma  Mu5000v, being the only mill guy in the shop she's all mine.

Link to comment
Share on other sites

This morning I roughed out the fines on the concave side of my part that I posted. Didn't really car for it, but it made it. I used a dynamic Opti rest rough off my stock model. 

I used a 3/16 .02 bull endmill. The dynamic motion ate me alive.  I would like to travel down thru there with 100 engagement depth of cut style. Any recommendation on toolpaths or different ways to use the one I am.

Link to comment
Share on other sites

What did you set the death of cut to? What plane did I you use rough the part? I will do a lot of 3+2 roughing aligning the plane to the best possible place. If the model where a solid I would have copied it to a level and dumbed it down using model prep to rough it with Multiaxis pocket. Even with an open shape you can cheat making some fence surfaces for the walls. I would approached the part completely different than you did. I would have laid it over if it fit in the machine and worked it that way verses standing up out of the vice. 

Those are great machines and you can do a lot with them. The 6300 with turning added is a nice machine. Get familiar with CALL0088 it is very powerful along with other parts of the OSP-300 control. Learn supernurbs and how to dial in the settings and filters for Mastercam and the machine, have a customer right now roughing 4140 ar 48rc at 200 ipm using Optirough and the Emuge Roughing tools. 

The insane part as you called it is at about 1400+ operations at this point. It is used for putting people and things into Space and has a very rigid set of programming requirements. 

Link to comment
Share on other sites

I would not use OPTI-ROUGH on those fins. I would waterline it to finish size and call it day. In case like this you will be a lot slower and never fully use the machine to it speed and feed doing it the way your trying to do it. Max RPM and .005 per tooth chip load with a finish step down and done. Part might move so if you are worried then leave stock doing a .05 to .1 step down to semi finish then come back and finish.  Might look at a taper ball endmill to have that shape made into a custom tool and then 2D contour it is another way. Time you have the tool made and finish the profile with a custom made tool you will come out ahead if doing production. If this is a one off then do the Waterline and call it a day.

  • Thanks 1
Link to comment
Share on other sites

Well after almost a full week of learning and trying new things, the money makers want parts faster. I'm now going to run in 2 vertical machines op1 an 2 style 2 parts each. Convex side 1st  with 4 work holes (1/4-20s) in the corners and .125 pin holes at the top of arc to locate on op 2. Thinking ill dish out an extra peace of stock so op 1 will sit rt in and off to the races (hopefully). I'm going to apply the toolpaths we discussed so id like to thank everyone for the pointer and hope to here from you in the future. Either way I had a lot of fun trying to make the five axis go. Ill get better over time ive got 25 years left so that should be plenty of time

Screenshot (11).png

Screenshot (12).png

Screenshot (13).png

Link to comment
Share on other sites
On 11/13/2020 at 6:31 PM, crazy^millman said:

Not to worry. I feel so honored to have your assistance. Its a brand new tool in my box. I do plan on playing with is part in my free time via hle of mastecam at home to make my vision real. Id like to play with your file from cam instructor but didnt have luck opening it in my HLE. Should i be able to open it?

 

Link to comment
Share on other sites
On 11/15/2020 at 9:24 PM, JB7280 said:

I was looking at the file that cncasylum posted, and got wondering, how the heck do you make a part, held like that, without a crazy amount of chatter?  I'm sure it works, because I see the method often, but it seems like the chatter would be unmanageable.

I was acually impressed wit rigidity. This big block when mounted was very ridged. In vertical position with indicator on the part i only saw .002 when pushing and pullin on it. I ran a 2 inch 4 flute facemill at .2 depth of cut .005 per tooth at 10000 rmps (200 ipm)and it loved it. My plan was to leave stock rails on left and right side with tabs that get cut off. But having to do the work on the front end first while rigid and working bk was a challenge for me. 

Link to comment
Share on other sites
12 hours ago, cncasylum said:

Not to worry. I feel so honored to have your assistance. Its a brand new tool in my box. I do plan on playing with is part in my free time via hle of mastecam at home to make my vision real. Id like to play with your file from cam instructor but didnt have luck opening it in my HLE. Should i be able to open it?

Yes if you have the 2021 HLE version I would think you should be able to open it.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...