Arched door molding

[john_hartman]

This is a continuation from my previous thread "arched top exterior door". I haven't started this project yet however I'm trying to familiarize myself with the "extruder" feature to mill the arched door molding. I am not making much progress and becoming more confused. I drew a simple profile to practice, but can't seem to get past this because there are open vectors and I can't close them to create a tool path. Do you create a V-carve, profile toolpath or a pocket toolpath? In B. Young's corner there is a nice 3D image. I assume this is the preview, but how do you get to this point? Has anyone done this who could provide some guidance? Many thanks!

[GlenP]

PRofile toolpath doesn't care about open vectors.

[john_hartman]

I was looking for a little bit more help than this... Thanks

[ghostcreek]

I am using the Aspire software, it has a two rail sweep function that works well for me. I am sorry to say I don't have any experience with the extruder feature. I would be happy to explain the two rail sweep to you if you like. If you figure out the extruder function, please share. It might take a bit of time for others to respond to your request. hang in there.

[GlenP]

Hey John, when using the "profile" toolpath you have to set it to cut "ON". Not inside or outside. Inside or outside try to go completely around as if closing the vector.
I usually draw up my design and then do a second layer in another colour for the toolpaths. You may have to make some offsets for your cutters to accommodate cutting "on". It takes some layout on paper and playing around to get exactly what you want. IF you have aspire you could do 2 rail sweep but I find it takes too long to cut.

[tkovacs]

First - I have never used the extruder - so I may be adding noise to this thread, but if I understand what the extruder is doing then the same could be done in aspire.

- create a surface using a 2 rail sweep.

- create a pocket toolpath over the surface and project it onto the surface.

[john_hartman]

Unfortunately I do not have Aspire. However, I made a lot of progress. I'm am able to create a curved door molding in the preview mode. Setting the tool path on "ON LINE" was the main problem, then not saving the toolpath in "inches" only was the other. Also, when creating a curved extrusion in partwork the length of the profile needs to be along the x-axis.

The next problem I'm contemplating is using a .5" ball nose bit. Using this size bit will not be able to get into a narrow gully or create a crisp line. Any thoughts on that one? Can two seperate bits be used? If so how?

[john_hartman]

Well I got my profile to preview just the way I want it, however the milling results are not even close. I've consulted Frank and he's duplicating my milling issues.

Since the profile tool path must be cut "on-line" the 1/2" ball nose bit cuts the perimeter dead-center on-line. Go figure. So a 2" wide-designed trim comes out at 1.5" wide. That's the first problem. The second problem is that the first past of the contoured portion of the profile goes down a 1/4" (the deepest part of the profile) then the rest of the profile cut is made over or doing air cutting. I can see that the profile is going through the proper form, just not in the wood. I could understand if it was doing an air cut for the entire profile, it would just be a "material thickness" and height adjustment. But I have a combination of material cutting and air cutting. I'm lost on this one. If anyone out there could lend a hand I would greatly appreciate it. I'll be sure to write an instruction sheet when this all gets figured out. thanks

[garyb]

John, if you want send me your dxf of the arc and profile and I will run it for you & send back in sbp.

[Gary Campbell]

John...
I have just completed a similar toolpath for a radiused shape that I need to cut on 250 decorative rafter tails next week. I barely know how to muddle thru this on my own, but will try to explain for you.

I set my profile on the exact x and Y coordinates that I want for my x and z. I have added a small negative line (.25")to make sure I have a negative z plunge at the end of file.

I do an OUTSIDE profile with my intended bit. I try a few different depth to get my desired results. The toolpath shown has a 1/2 bit diameter depth. Save toolpath using "inch" not arcs postP.


5071

I open the SPB file saved and maually edit out the portions of the file between the red lines. This takes a little practice, but if you are careful with placement, position becomes very obvious.

Once this editing is done I send to extruder. The extruder has not returned predictable results to me, most likely thru inexperience, especially as it relates to existing Y coordiates transformed into Z heights. It usually takes me a few trys to get the X and Y coordinates that I want.

After an hour of trial and error I have the file I need, which will cut the notch and radiused end on twelve 4 by 6 rafter tails side by side with the 6" face vertically oriented.

Due to the height I have hand coded lead ins, lead outs and single axis moves to park the bit out of the way for table loading. Hope this helps.

5072
Gary

[Gary Campbell]

John...
I went over to "the Dark Side" and talked to Bill Young, who wrote the extruder program. I found that I was experiencing unpredictable results due to using PartWizard software. I have switched to PartsWorks (VCarve) and here is how to do it.

Place your part oriented as above. Selecting an ENDMILL that is the same diameter as the ballnose you plan to cut with, do an outside/right or inside/left toolpath .010 deep with a climb/conventional option that gives you a toolpath around your profile in the direction that you desire.

Save this toolpath using the "inch" postP.

Start the extruder and extrude this SBP file with the parameters you require.

I found this much easier to accomplish using Vectric than Delcam software, but other than the ability to do an outside profile on an open vector, dont know why.

Here is a screenshot of a proper toolpath that doesnt need editing from PartsWorks:

5073

[john_hartman]

Thanks Gary B. I may take you up on this, but I would really like to learn how to do this.

Thanks Gary C. I have read your explanation and still need to study it a bit more. I read Bill Youngs extruder tutorial on his "Corner" as well. Which is exactly how I got the extruder to work to this point in preview mode. It just doesn't mill the same way at all.

The one thing that catches my eye. Is creating the toolpath outside or inside the line. This was the very first problem I encountered. I could only get the profile to toolpath by selecting "on-line". But this is now the problem. How can you toolpath outside or inside on an open vector?

[garyb]

"How can you toolpath outside or inside on an open vector?"

You can create 2d profile toolpath on an open vector, then select which side of the line to cut and of course direction.

[bill.young]

John,

I missed this thread while I was in California but Gary Campbell pretty much covered it in his last post...it's pretty straightforward. You have to create the toolpath "above" the profile using the same size endmill as the ballnose bit that you'll be cutting with, in order for the size to end up correct.

What version of PartWorks do you have? I seem to remember that the first version didn't let you do outside and inside toolpaths on an open vector, but it was added in the next version (1.1 maybe?).

The other thing that can be tricky is getting the toolpath "above" the profile and going in the right direction. I usually end up having to try it with Inside, Outside, Climb, and Conventional until it's the way that I want it.

Bill

[john_hartman]

Bill,

It's version 1.007, built Nov. 5, 2007. Is this my problem?

Thanks,

John

[john_hartman]

Bill,

Assuming my version is the issue how did you get the extruder to work in March of 06? I've tried every combination of outside/inside profile toolpath with no luck. I just get "1 open vector". Also, when I eventually get the path to save how do I know if the toolpath is going in the right direction?

Incidentally I'm just practicing with a random drawn profile. It's not the actual piece I will be cutting, as I don't know what it will be yet. Is there a limitation to the amount of detail which can be extruded?

[Gary Campbell]

John...
Bill will probably chime in and let you know the easier method, but the 1st version I described is the way I did it before the software added the features that you seem to be missing.

The amount of detail you can cut is limited to what can be cut with your selected bit diameter. The trade off is time. As you add detail, you add passes to get the detail and therefore add time.
Gary

[john_hartman]

Gary, realizing that I may screwed with the older version I have been studying your first post. A couple of questions: 1) is your 0,0 on the lower left hand corner? 2) How did you manually edit out the unwanted portions? I tried doing this with the "substrate vectors" icon. I guess this is part about practice, but I'm not even close...

[Gary Campbell]

John...
1) Using a casing profile as an example, I would orient the bottom of the molding at X=0 if I was going to extrude in the X direction and at Y=0 if I was going to extrude in the Y.

2) When I speak of manually editing out the unwanted portions of the file, I am removing unwanted lines of an outside profile toolpath in the saved SBP file. As long as you can be aware of the molding size, location and the bit diameter, this will take a little math and a few minutes. After a couple tries, it becomes easier. If you were going to do this very often, I would recommend a software upgrade.
Gary

[bill.young]

Hi John,

I don't know when that ability was added but I'll try to find out...an email to ShopBot would probably be quicker though and you can also find out about upgrades if that's the issue.

As far as I know there's no easy workaround...Gary's manual editing after toolpathing a closed vector is the only way I know of but isn't an easy solution.

Bill

[bill.young]

I don't have your version installed so can't tell for sure, but this might be the update that added that ability.

http://www.shopbottools.com/drivers.htm

(it's the first thing listed)

Bill

[john_hartman]

Bill,

Thank you so much for the drivers link. I downloaded version 1.102 and can now tool path an open vector. I haven't tried the extruder yet, but I suspect that it will work much better... Cheers!

[geometree]

I've been using the extruder a bit and have it working except for the multiple passes. How does that work? Nothing I do seems to make a change in the maximum depth of cut. Thanks

[Gary Campbell]

Guys...
Got around to cutting these today. Gnarly ol' pressure treated decorative rafter tails. Over 250 to cut, 13 at a time with the extruded file shown above in preview. A year ago I wouldn't let the green stuff touch the Bot. Gotta pay bills now. Here is a batch just cut.

5074
Gary

[john_hartman]

Gary, those look like 2x6's..!? Just how long was that bull-nose bit?

I found that the first pass likes to plunge to the deepest/lowest level then cut across. So I need a bit which is the material thickness plus some otherwise the shank will make contact with the .75" material. (The cutting edge of the bull nose I had on hand was only .5" tall) Good thing I tested this on a tacked down piece of MDF!

I haven't tried this yet but since a bull nose bit will leave a radius and not a nice crisp sharp edge I was wondering if a v-carve bit of the same diameter as the specified bit in the parameters would be able to get into the "finer" lines of moldings and such? Any thoughts on that.

[Gary Campbell]

John...
Actually they are 4 by 6's, and fine cabinet lumber, too. Ballnose is 4" long with 3.25" below collet. cutting at 6ips with .05 +/-stepover.

5075

I cant help much with the pro's and cons of 3D cutting as I dont do much, if any. I am sure that the more knowledgeable will chime in.
Gary

[wberminio]

Gary

I couldn't see those cut any simpler way.
Must smell sweet!
Just Imagine your cutting 4x6 cherry.

Erminio