Site Logo
Site Logo
 
It is currently Mon Mar 27, 2017 11:12 am

All times are UTC




Forum locked This topic is locked, you cannot edit posts or make further replies.  [ 7 posts ] 
Author Message
 Post subject: Facemill on an ARC
PostPosted: Fri Dec 11, 2015 6:26 pm 
Offline

Joined: Wed Jun 03, 2015 11:46 am
Posts: 9
Hello,
Please see attached picture.

I am trying to mill the face outlined (poorly) in red using a 3" facemill. We have a clamping device in the center of this part that is not shown. When I select "mill face" feature in featurecam the tool patch is square ie (the tool machines begins on the right and moves straight down, steps over to the left a certain distance, moves straight up, moves over to the left a certain distance etc). The problem is this tool path (and most others I have tried) run into our clamp.

What I would like is for the facemill to follow the path of the arc. I have tried setting boundaries and have had no luck. Anyways, the green arrow is pointing to the inner most diameter the facemill would have to follow.
Attachment:
Pic1.png
Pic1.png [ 120.6 KiB | Viewed 2131 times ]

I can program it by hand but I need to figure this out in featurecam for future projects. I need to be able to do this in the program.
Please help me out, I have already spent too much time on this one feature.


FC 2015 x64


Top
 Profile  
 
 Post subject: Re: Facemill on an ARC
PostPosted: Mon Dec 14, 2015 1:45 pm 
Offline

Joined: Thu Oct 03, 2013 3:51 pm
Posts: 33
Location: Right Here
Have you tried right clicking on a clamp solid and selecting "use solid as a clamp"? I've never had an occasion where I needed to do that, but I imagine that it should work.


Top
 Profile  
 
 Post subject: Re: Facemill on an ARC
PostPosted: Mon Dec 14, 2015 2:37 pm 
Offline

Joined: Wed Jun 03, 2015 11:46 am
Posts: 9
Yes I have selected the clamping device as such in featurecam and still did not get the result I was looking for.


Top
 Profile  
 
 Post subject: Re: Facemill on an ARC
PostPosted: Mon Dec 14, 2015 9:04 pm 
Offline

Joined: Sat Mar 10, 2007 6:23 am
Posts: 270
Location: S.F. Bay Area
If you use a groove feature insted of the face feature your toolpath becomes less limited but it's a bit more work. You have to create the centerline for the toolpath yourself. In this case offset the arc where you have the green arrow pointed by 1.5" towards the outside (1.3" is porbably better to make sure the facemill cleans up along inside of the entire arc). You also have to add a lead-in/lead-out at least 1.5" below your bottom edge of the part so the facemill doesn't plunge into the part. Create a curve from these 3 segments. Select the curve and create a "simple groove/engrave" feature. Make the Width 3.0 and set the depth to say .050 (or whatever stock thickness you want to remove). In the LOCATION tab put +0.050 so the bottom of the groove will end at Z=0.000 (different from the face feature!!!).
You can reverse the cut direction by going to the STRATEGY tab and selecting "reverse curve". If you want to do multiple rough passes, make the depth and location larger (maybe both 0.4") and select a "Rough Pass Z-increment" (0.1" for example).

Play around with the shape of your curve and all the other settings and if you have more questions, search the forum for more post on the same subject.


Attachments:
Untitled-01.png
Untitled-01.png [ 124.06 KiB | Viewed 2089 times ]
Top
 Profile  
 
 Post subject: Re: Facemill on an ARC
PostPosted: Mon Dec 14, 2015 9:48 pm 
Offline

Joined: Wed Jun 03, 2015 11:46 am
Posts: 9
Attachment:
View1.png
View1.png [ 129.47 KiB | Viewed 2069 times ]


Worked like a freaking charm! Thanks man! I have so many other questions, please look them over if you can, I am a little in over my head and I am trying to use learn Featurecam as I go.


Top
 Profile  
 
 Post subject: Re: Facemill on an ARC
PostPosted: Tue Dec 15, 2015 1:21 am 
Offline

Joined: Thu Feb 14, 2013 2:49 am
Posts: 93
Location: Seattle, WA
Your speed and feed for the 'groove' will also be different than 'face'


Top
 Profile  
 
 Post subject: Re: Facemill on an ARC
PostPosted: Tue Dec 15, 2015 1:45 am 
Offline

Joined: Thu Jan 18, 2007 6:24 am
Posts: 358
Location: CT
Yupp, groove feature is awsome for this kind of stuff, but there is only one caveat.
Don't know about the most recent release, but in previous versions you had to have a tiny bit
of material to remove in the "groove" feature, otherwise no toolpath will be created.

Simple enough of a workaround though, as you can enter as little as .0001 for depth.


Top
 Profile  
 
Display posts from previous:  Sort by  
Forum locked This topic is locked, you cannot edit posts or make further replies.  [ 7 posts ] 

All times are UTC


Who is online

Users browsing this forum: No registered users and 6 guests


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
Powered by phpBB